## CATIA Surface Design .fr

Sep 19, 2008 - Present the different Companion documents available for additional information and the ..... operations in the tree structure) and a Geometrical Set (Wireframe ... use of a Geometrical Set is for creating logical organizational.
Surface Design

CATIA V5 Training

Foils

CATIA Surface Design

Instructor Notes:

Version 5 Release 19 September 2008 EDU_CAT_EN_GS1_FI_V5R19

Surface Design

Upon completion of this course you will be able to: - Identify and use the tools specific to the Generative Shape Design workbench - Create simple reference and Wireframe geometry - Use the reference wireframe elements to create simple surfaces - Create clean topology from a set of surfaces and smooth sharp edges - Detect and correct the discontinuities on curves and surfaces - Create solids from surfaces

Targeted audience

Mechanical Surface Designers

Prerequisites

Students attending this course should be familiar with the CATIA V5 interface.

Instructor Notes:

1 Day

Surface Design

Table of Contents (1/4) Introduction to Surface Design Introduction to Surface Design The Generative Shape Design Workbench Surface Design Workbench User Interface Surface Design Workbench Terminology Surface Design Workbench General Process

Creating Wireframe Geometry Why Create 3D Wireframe Geometry ? Creating Points in 3D Creating Lines in 3D Creating Planes in 3D Creating Curves in 3D Creating Wireframe Geometry: Recap Exercises Additional Reference Material To Sum Up

Shape Design Common Tools Why Use Common Tools ? Stacking Commands

Instructor Notes:

7 8 9 12 14 15

16 17 18 21 25 30 36 39 40

41 42 44

Surface Design

Creating Surfaces Why Create Surface Geometry ? Creating Basic Surfaces Creating a Swept Surface Creating a Surface Offset from a Reference Creating a Surface from Boundaries Creating a Multi-Section Surface Creating Basic Surfaces: Recap Exercises Additional Reference Material To Sum Up

Performing Operations on the Geometry Why are Operations on Geometry needed ? Joining Elements Splitting/Trimming Creating Fillets Transforming Elements

Instructor Notes:

52 58

59 60 61 67 76 79 86 102 105 106

107 108 110 114 123 131

Surface Design

Completing the Geometry in Part Design Why Complete the Geometry in Part Design ? Creating a Solid from Surfaces Completing Geometry Recommendations Completing the Geometry in Part Design: Recap Exercises Additional Reference Material To Sum Up

Modifying the Geometry What about Modifying the Geometry ? Editing Surface and Wireframe Definition Modifying Geometry Recommendations Modifying the Geometry : Recap Exercises

Instructor Notes:

137 141 143 159 162 163

164 165 166 171 173 176 177

178 179 180 183 186

Surface Design

Using Tools What about Using Tools ? Creating Datum Features Checking Connections Between Elements Updating a Part Using Tools: Recap Exercise Additional Reference Material To Sum Up

Master Exercise: Mobile Phone

Mobile Phone: Presentation Mobile Phone (1): Creating Wireframe Geometry Mobile Phone (2): Creating Basic Surfaces Mobile Phone (3): Trimming and Joining the Body Surfaces Mobile Phone (4): Creating the Part Body Mobile Phone (5): Modifying the Geometry

Instructor Notes:

189 190

191 192 193 195 198 202 203 204

205 206 207 208 209 210 211

Surface Design

Introduction to Surface Design The Generative Shape Design Workbench Surface Design Workbench User Interface Surface Design Workbench Terminology Surface Design Workbench General Process

Instructor Notes:

Surface Design

Introduction to Surface Design The creation of wireframe and surface geometry is often needed to define the complex shapes of parts. Ultimately we want to create a solid to best capture our design intent, however this model may include surface geometry integrated into the solid part. Later, we will take a more in depth look at the shape design process, but for now it is important to consider the key points.

Key Points

Wireframe and surface geometry is used to define more complex 3D shapes in the design process. Wireframe, surface and solid geometry form an integrated set of modeling capabilities that allow us to capture the design intent.

Wireframe geometry Surface geometry Solid geometry

Instructor Notes:

Explain that often we need all the tools: wireframe, surface and solid geometry to accurately capture the design. Solid geometry has a limitation on its own, but integrated with surfaces, more complex shapes can be defined. Emphasize the Key Points on this slide to the students. Point out that the association between wireframe, surfaces and the solid part is maintained. Changes in shape geometry can be updated in the solid part. Guide the students in the progression from wireframe to surfaces to solids as shown in the images for the mouse exercise. You can mention that the students will be creating this mouse part.

Surface Design

The Generative Shape Design Workbench (1/3) Generative Shape Design workbench has a wide functional set. It is a complete surfacing tool used to create complex shape parts.

With Generative Shape Design workbench, designers can easily design surfaces of plastic parts or shells. After importing some surfaces the designer can check and heal them with the CATIA - Healing Assistant 1 (HA1) product. He can then modify and add other surfaces using powerful wireframes and surfaces creation tools of GS1.

To finish, the design parts will be manufactured after the surface machining programming in the CATIA 3-Axis Machining 2 (SMG) product.

Instructor Notes:

This slide has general information . You can quickly move through this slide.

Surface Design

The Generative Shape Design Workbench (2/3) CATIA - GSD provides a comprehensive set of features for shape design. These include wireframe elements like: Point, Line, Plane, Curves, Circle. Spline, Parallel curves, 3DCorner , Connect curve, Spiral, Intersection and Projection.

Standard and advanced surface features include:

Extrude, Revolute, Sweep and Fill. Standard combinations of elements use associative transformation, such as Symmetry, Scaling, Translation, Affinity, Extrapolation and Fillet.

Instructor Notes:

This slide has general information . You can quickly move through this slide.

Surface Design

The Generative Shape Design Workbench (3/3) Associative Design : Design in context allows concurrent work with user control of associativity. The wireframes and surfaces can be designed using the part or assembly context. When design changes are made, the user controls the propagation of modification.The designer can reuse an existing surface, and link in additional parts to support concurrent engineering.

Several Generative Shape Design features help for efficient management of design modifications.

A datum curve or skin used in one feature can be replaced. A set of features can be isolated as a single feature (with no history) to facilitate design comprehension and accelerate design changes.

Instructor Notes:

This slide has general information . You can quickly move through this slide. Now to the Show me… (The show me in the user Companion after this slide takes a walkthrough for the generative shape design workbench and tries to highlight some of the possibilities)

Surface Design

Surface Design Workbench User Interface (1/2) Workbench Icon

Specification Tree

Sketcher access...

Shape Design tools...

Containers of type Geometric Set , Ordered Geometric Set and Body

Standard tools

Instructor Notes:

This area shows current status

Command Bar

Surface Design

Surface Design Workbench User Interface (2/2)

Instructor Notes:

Surface Design

Surface Design Workbench Terminology Part is a combination of Part Body and Geometrical Sets. PartBody basically contains the features used to create a solid. It can contain surfacic and wireframe elements also.

If you create Reference Elements ; points, planes, lines in Part Design Workbench , you have the option of directly containing them in Part body / Body , or you can insert a Geometric set and place these elements.

Geometrical Sets contain the features used to create surface and wireframe elements. Ordered Geometric Sets(OGS) contain surface and wireframe . The elements in this body are created in a linear manner. OGS can also contain “Body” . Body allows creation of Part Design Solids within an OGS.

“Body” can be inserted in OGS to contain Part Design Solids.

When you enter the Generative Shape Design workbench Part Body is the default body available. “Geometric Set”, “Ordered Geometric Set” can be inserted manually.

Instructor Notes:

Surface Design

Surface Design Workbench General Process 1

Enter the Generative Shape Design workbench

Enter the Part Design workbench

3

4

Instructor Notes:

Create the surfaces Trim and join the body surfaces

Create the part body

5

Modify the geometry

Create the wireframe geometry

2

Surface Design

Creating Wireframe Geometry You will become familiar with the creation of wireframe geometry elements

Why Create 3D Wireframe Geometry ? Creating Points in 3D Creating Lines in 3D Creating Planes in 3D Creating Curves in 3D Creating Wireframe Geometry: Recap Exercises Additional Reference Material To Sum Up

Instructor Notes:

Surface Design

Why Create 3D Wireframe Geometry ? In many design situations, there is a need to create geometry that is defined using the entire 3D space. This geometry is not limited to a single plane and therefore can not be defined using the Sketcher workbench. These elements including points, lines, planes and curves created in 3D space are called Wireframe geometry. Wireframe geometry is used primarily as construction geometry for creating more complex 3D elements such as curves and surfaces.

Key Points

Wireframe geometry and Sketch geometry can be used together in defining more complex 3D elements.

Even though Wireframe geometry is created in 3D, a support element (plane or surface) may be required to define the geometry.

Wireframe geometry

Surface geometry

Instructor Notes:

Explain the Key Points outlined in this slide. Emphasize that Wireframe geometry and Planar geometry from Sketches can be used in concert to develop Surface and/or Solid geometry features. Note that Wireframe geometry can also be Planar when its Support is planar. Wireframe geometry that is created with a Planar support can be used for generation of many other features that require a Profile (typically defined as a Sketch) as input.

Surface Design

Creating Points in 3D

You will learn the different ways to create points in 3D

Instructor Notes:

Surface Design

Why Do You Need Points ? To support creation of all geometrical elements and to use them as reference for any creation.

Identification in tree

Coordinates

- A point can be defined by its coordinates from a reference point (origin or selected point). - A point can be defined with respect to an element. You can edit any type of point by double-clicking on its identifier in the tree or on the geometry. You will then change its specifications in the Point Definition box.

Default color codes for points: On plane

. Blue for point or projection of point in creation . White when created . Green for reference

Between

On curve

In some cases you can reverse the direction of creation of the point, clicking either the red arrow on point or the Reverse Direction button in the Point Definition box.

Instructor Notes:

Explain why you need Points in Wireframe development. Describe how Points are fundamental position controls for a wide variety of elements. Note the Tree and Geometry Views for how Points are displayed during and after creation.

Surface Design

Creating Points Point types available in the Generative Shape Design workbench (MD2 license):

Type

Description

Point by Coordinates

Create a point by defining its coordinates in 3D.

Point on a Curve

Create a point on a curve at a distance from a reference point.

Point on a Plane

Create a point on a plane at a distance from a reference point.

Point on a Surface

Create a point on a surface at a specified distance and direction from a reference point.

Point at a Circle/Sphere Center

Create a point at the center of a circle/Sphere.

Point Tangent on a Curve

Create curve tangent points for a specified direction.

Point Between Two Points

Create a point between two existing points using a ratio value.

Points Spaced on a Curve

Create several points equally spaced on a curve

Instructor Notes:

Demonstration is needed on these points. Coordinates On plane On curve

Surface Design

Creating Lines in 3D

You will learn the different ways to create lines in 3D

Instructor Notes:

Surface Design

Why Do You Need Lines ? (1/2) You can use lines as guide, reference, axis, direction or join to create other geometric elements.

What about lines ? Identification in tree Point-Point PointDirection

A line can be created: from points or vertices* on a curve on a support

You can edit any type of line by double-clicking on its identifier in the tree or on the geometry. You will then change its specifications in the Line Definition box. You can lock the ‘Line type’ submenu by clicking on this icon.

Angle/Normal to curve

Tangent to curve

This option allows you to create the line on a support surface.

You can restrict the length of the Line by selecting an element in Up-to 1 or Up-to 2 fields.

Normal to surface

Instructor Notes:

Highlight that lines can be used as tangency directions for splines, extrusion direction or guide curves, or sections for sufaces, etc… Lines lying on a support surface could be used to split the surface.

Surface Design

Why Do You Need Lines ? (2/2) Modification of line parameters (length, orientation) Graphic manipulators

You can reverse the direction of creation of the line by either clicking the red arrow on line origin or the Reverse Direction button

Line origin

Instructor Notes:

Explain methods of adjusting the Length of a Line using dialogue box values or by dragging and dropping Graphic Manipulators in Geometry view. Note that for certain line types you can Reverse Direction if it is not in the direction you wish.

Surface Design

Creating Lines Line types available in the Generative Shape Design workbench (MD2 license):

Type

Geometry

Description

Line Between Two Points

Create a line between two selected points.

Line from a Point and Direction

Create a line based on a reference point and a specified direction.

Line at an Angle or Normal to a Curve

Create a line at an angle to a curve that passes through a point.

Line Tangent to a Curve

Create a line tangent to a single curve, a point and a curve, or two curves.

Line Normal to a Surface

Create a line normal to a surface at a selected point.

Bisecting Line

Create a line that splits the angle between two lines into equal parts.

Instructor Notes:

Make a demonstration to the students for: Line at an Angle or Normal to Curve Line tangent to a Curve.

Surface Design

Creating Planes in 3D

You will learn the different ways to create planes in 3D

Instructor Notes:

Surface Design

Why Do You Need Planes ? You can use planes as reference elements to create new geometry or as cutting elements.

What about planes ? You can create a plane from: another plane

Identification in tree

points, lines or curves

Offset Angle/Normal to plane

its equation

Through 3 points

Equation

Instructor Notes:

Explain why you might need to create planes to support your development of a Wireframe and Surface design. Point out that planes are also used in the development of Solid features in Part Design.

Surface Design

You can restrict automatic change of ‘Plane type’ submenu by clicking on the Lock button. In some cases you can reverse the direction of creation of the plane, clicking either the red arrow on plane origin or the Reverse Direction button in the Plane Definition box.

Graphic manipulator

Plane origin

You can modify the plane offset keying in the offset value in the Plane Definition box or dragging the graphic manipulator.

Instructor Notes:

Explain that similar operations as covered in for Line creation are available for Plane creation: Reverse Direction, Graphic Manipulators for drag and drop postioning, Distance key-in from a dialogue box.

Surface Design

Creating Planes

(1/2)

Plane types available in the Generative Shape Design workbench (MD2 license):

Type

Geometry

Offset Plane

Parallel Plane through a Point

Description Create a plane parallel to a reference plane offset at a distance. Create a plane parallel to a reference plane through a point.

Plane at an Angle or Normal to a Plane

Create a plane at an angle to a reference plane based on a rotation axis.

Plane through 3 Points

Create a plane passing through 3 points.

Plane through 2 Lines

Create a plane passing through 2 lines.

Plane through a Point and a Line

Create a plane passing through a point and a line.

Instructor Notes:

The following important types of line types can be shown to the students. Plane parallel through a point Plane at an Angle or Normal to a Plane.

Surface Design

Creating Planes

(2/2)

Plane types available in the Generative Shape Design workbench (MD2 license):

Type

Geometry

Description

Plane through a Planar Curve

Create a plane passing through a planar curve.

Plane Normal to a Curve

Create a plane normal to a curve at a specified point.

Plane Tangent to a Surface

Create a plane tangent to a surface passing through a specified point.

Plane by an Equation

Create a plane by defining the components of the equation of the plane.

Mean Plane through Points

Create a plane defined as the mean through 3 or more points.

Plane Spaced Between 2 Planes

Create several planes spaced equally between 2 selected reference planes.

Instructor Notes:

The following important types of line types can be shown to the students. Plane Normal to a Curve Plane by an Equation.

Surface Design

Creating Curves in 3D

You will learn the different ways to create curves in 3D

Instructor Notes:

Surface Design

Why Do You Need Curves ? You can use curves as guide or reference to create other geometric elements or as limits of a surface.

What about curves ? A curve can be created from: points, other curves or surfaces

A spline is a curve passing through selected points with the option to set tangency conditions at its extremities.

You can edit any type of curve by double-clicking on its identifier in the tree or on the geometry. You will then change its specifications in the corresponding definition box.

Instructor Notes:

Highlight the different types of curves: Tell the students that they can also create their own composite curves(for example, a line and another element such as a spline can be joined together).

Surface Design

Creating Curves (1/4) Curve types available in the Generative Shape Design workbench (MD2 license):

Type

Geometry

Projection Curve

Intersection Curve

Circle

Description Create a curve by projecting an existing element onto a plane or surface.

Create a curve defined by the intersection of existing elements.

Create a complete or partial circle defining parameters such as center, radius, and tangency.

Corner

Create a rounded corner of a specified radius between 2 elements.

Instructor Notes:

Demonstration required for : Projection Curve Intersection Curve

Surface Design

Creating Curves (2/4) Curve types available in the Generative Shape Design workbench (MD2 license):

Type

Geometry

Parallel Curve

Reflect Line

Connect Curve

Description Create a curve that is parallel to an existing curve at a specified offset distance.

Create a curve defined by point locations of all surface normal at specified angle.

Create a curve that will connect 2 existing elements.

Conic Create a conic curve of the type parabola, hyperbola or ellipse.

Instructor Notes:

Demonstration required for : Projection Curve Intersection Curve

Surface Design

Creating Curves (3/4) Curve types available in the Generative Shape Design workbench (MD2 license):

Type

Geometry

Spline

Description Create a curve passing through points on which you can impose tangency conditions.

Helix Create a helical curve oriented by an axis.

Spiral

Create a spiral curve defined on a support plane.

Polyline

Instructor Notes:

Demonstration required for : Connect Curve Spline

Create a single element consisting of multiple line segments.

Surface Design

Creating Curves (4/4) Curve types available in the Generative Shape Design workbench (MD2 license):

Type

Geometry

Isoparameteric Curve

Combine Curve

Instructor Notes:

Demonstration required for : Connect Curve Spline

Description Create a curve from the isoparameters of a surface.

Create a 3D curve by combining two planer curve lying on a different planes.

Surface Design

Creating Wireframe Geometry Recap Exercises 25 min

Button Mouse

Instructor Notes:

Surface Design

Creating Wireframe Geometry Recap Exercise: Button 10 min 3D Line

In this recap exercise you will create: Points in 3D Lines in 3D Spline in 3D Sketches Spline

3D Points

Instructor Notes:

Sketches

Surface Design

Creating Wireframe Geometry Recap Exercise: Mouse 15 min

In this recap exercise you will create: Points in 3D Wireframe Circle 3D Spline Intersections and Projections

Instructor Notes:

Surface Design

Additional Reference Material Additional information can be found in the following reference material: Companion: Skillets: Creating Points in 3D, Creating Lines in 3D, Creating Planes in 3D, Creating Curves in 3D

Keywords: Point, Line, Curve, Plane

Documentation: Books:

Mechanical Design Solution – Wireframe & Surface Design Shape Design Solution – Generative Shape Design

Search String:

Point, Line, Plane, Curve, Circle, Conic, Spline, Projection, Intersection

Instructor Notes:

Present the different Companion documents available for additional information and the on-line documents. NOTE: a demonstration is preferred to assist the students in locating the documents and showing at least one of them. It should be stated that these sources of documentation do a go job in covering the features.

Surface Design

To Sum Up ...

You have seen CATIA V5 – Creating Wireframe Geometry: How to create points using different methods like point using co-ordinates, on a curve, on a surface, on a plane, point between two points … How to create lines using different methods like line between two points, line from a point and direction, line tangent to a curve … How to create planes using different methods like plane offset to a plane, plane through three points, plane through two lines …

How to create curves using methods like Projection, Reflect line, Intersection, Parallel, Corner, Spline, Helix, Spiral …

Instructor Notes:

Surface Design

Shape Design Common Tools You will become familiar with the shape design common tools

Why Use Common Tools ? Stacking Commands Managing Geometrical Sets To Sum Up

Instructor Notes:

Surface Design

Why use Common Tools ? (1/2) There are many tools that can be accessed during the shape design process that are not dependant on the type of element being created. We refer to these tools as Common Tools. Before we explore more about creating shape elements, it is important to understand how two critical common tools can be used in our design process.

Key Tools

Stacking Commands

Geometrical Sets

Instructor Notes:

Surface Design

Why use Common Tools ? (2/2) Common tools are used to increase productivity in the shape design process. Stacking Commands - allow you to create additional “construction” geometry without interrupting the primary element creation task. The design process is more efficient when stacking commands: - No need to change from one command icon to another. - Stacking commands are presented in context of the primary task. - Design flow is clearly displayed as running commands.

Geometrical Sets - allow you to organize shape geometry in the tree to more clearly capture design specifications. The CATIA part is easier to manage and manipulate downstream:

- Objects can be located quickly under renamed Geometrical Sets. - Objects can be easily moved and reordered between bodies.

Instructor Notes:

Explain the use of Stacking Commands at the advantage of being able to create Support Geometry for a given feature “on the fly” via contextual menus. Point out that a Running Commands dialogue box is automatically opened when you enter into this mode. Explain what Geometrical Sets are and how they differ from Part Bodies. Note that where solid features in Part Bodies have an order of operation that affects the resultant solid, Open Bodies have no order of operation and are used to organize Wireframe and Surface Geometry.

Surface Design

Stacking Commands

You will learn how to stack commands while creating wireframe elements.

Instructor Notes:

In this section, we will look at how to use Stacking Commands while creating Wireframe and Surface elements. Note that Stacking Commands is also available while creating Part Design solid features and elsewhere in CATIA V5.

Surface Design

Why Do You Need to Stack Commands ? Stacking commands allows you to create construction elements while creating an element which requires those construction elements.

You can create the following construction elements: - points, - planes, - intersections, - extracts. - lines, - projections - boundaries, You have access to the stacking commands capability while creating: - points, - circles, - translations, - splines, -extrudes, - lines, - conics - rotations, - helixes, -sweeps, - planes, - corners, - symmetry - spirals, -blends.

Using mouse button 3 you display a contextual menu listing all the elements you can create using the stacking commands capability.

Stacking command facility is available in almost all the GSD commands.

Instructor Notes:

Explain the advantage of using Stacking Commands to create support geometry for a Feature without having to close that Feature’s creation dialogue box. Note the types of Wireframe features that provide contextual access to Running Commands and the types of support elements that can be created through that access.

Surface Design

Stacking Commands… While creating an element you may need a construction element that you will create on the fly.

You define the parameters of the construction element.

When using the stacking command capability you can check the status of the stack in the Running Commands window.

The construction element is created and selected at the same time.

Instructor Notes:

Explain how Stacking Commands are accessed through contextual menus for support geometry creation. Point out the flow of this process and how it relates to the Running Commands dialogue box that is automatically opened. Note that Running Commands can “tree down” through many levels if necessary.

Surface Design

Tree Organization for “Stacked Commands” Features created on the fly (using stacking commands) are owned by the creating feature. These features are aggregated in the tree right under their parent feature: This series of stacking command will lead to this tree:

Construction elements created using the stack facility are created in no show mode in the specification tree.

Instructor Notes:

Point out that when skacking commands, these features are placed under the parent feature as shown to the right.

Surface Design

Stacking Commands (1/4) When you create some wireframe elements (point, line, plane, circle, corner, conic) or when you perform a translation, a rotation or a symmetry on an object you can create on the fly the missing construction elements, i.e. points, lines, planes, intersections or projections. In the following example you will see how to create a plane from scratch.

1

2 Select the type of plane you want to create.

3 Using mouse button 3 click in the Point Copyright DASSAULT SYSTEMES

field and select the Create Point option. The Point Definition window is displayed.

Instructor Notes:

In the example of creating a Plane through a Point and a Line, you will need to define the Point and Line in order to complete the Plane creation operation. If this required geometry does not already exist, you can access the tools to create them directly from the Plane Definition dialogue box by using the Contextual Menus available.

Surface Design

Stacking Commands (2/4)

4 Define the parameters to create the point.

The status of the stacking commands is also displayed in the Running Commands window.

5 Click OK to accept point creation.

The Plane Definition window is displayed again with Point.1 in the Point field. The Point button next to the

Point field allows you to edit the point parameters.

6 Using mouse button 3 click in the Line

field and select the Create Line option. The Line Definition window is displayed.

Instructor Notes:

In this example, you can create the necessary support Point needed to create the Plane. Note the Running Commands dialogue box describes where you began and where you currently are in the Stacking Commands process. Point out that support features can also be edited through Running Commands wether or not they were initially created through Stacking Commands.

Surface Design

Stacking Commands (3/4)

7 Define the parameters to create the line.

The status of the stacking commands is also displayed in the Running Commands window.

8 To create the points needed for the

line you can also use the stacking commands. In that case the Running Commands window will look like this:

Instructor Notes:

Explain the process where the Plane requires a Line. The Line definition dialogue box is accessed through Running Commands. The Line requires a Point for its definition. This is also created using Stacking Commands via the Contextual Menu. Point out the Running Commands dialogue box hierarchy. Note that if the Point required geometry that is not in existence, a contextual menu could tree the Running Commands down even further.

Surface Design

Stacking Commands (4/4)

9 Once the two points are created click OK

to accept the line creation. The Plane Definition window is displayed again with Line.1 in the Line field. The Line button next to the Line field allows you to edit the Line parameters.

10 Click OK to accept the plane creation.

If you want to modify a parameter of the plane you can also double-click on its identifier inLine.1 the specification tree.

Instructor Notes:

Explain how once you have returned to the original geometry creation dialogue box from which Stacking Commands was invoked, all required support geometry has been defined. Note how clicking OK will not only finalize creation of the desired Plane (in this example), but also will finalize creation of all the support geometry created through Running Commands. Point out that the geometry created using Stacked Commands will be located under the parent in the Specification Tree.

Surface Design

Managing Geometrical Sets

You will learn how to insert and select a Geometrical Set and how to manage the elements belonging to a Geometrical Set.

Instructor Notes:

In this section, you will learn what a Geometric Set is and how to create one and manage its contents…

Surface Design

Why Do You Need Geometrical Sets ? Geometrical Sets are containers for wire frames and surfaces. They are useful to show clearly the part’s detailed structure. They function as folders where you store and group your features. Using Geometric sets you can multi-select all the elements in operations where multi-selection is allowed.

• In Generative Shape Design workbench you can insert a ‘Geometrical Set’ from Insert Menu. • You can create as many ‘Geometrical Sets’ as you need. • Once you make a ‘Geometrical Set’ current, the next created wire frames or surfaces will belong to it. • You can move elements from a ‘Geometrical Set’ to another.You can also move elements within a “Geometric set” . Moving elements within a “Geometric Set” does not change the geometry created.

Current Set (underlined): to define a Geometrical Set as ‘current’ : - click on it with mouse button 3 and selecting ‘Define in Work Object’, - select it in the body selector available in the Tools toolbar. Elements belonging to the Geometrical Set.3

Instructor Notes:

Explain the primary differences between a Part Body (Solid features with an order of operations in the tree structure) and a Geometrical Set (Wireframe and Surface features with no order of operations in the tree structure). Point out that the primary use of a Geometrical Set is for creating logical organizational structures for Wireframe and Surface elements in the Tree View. Also mention to the students about the new Hybrid capability of Part Body , which is called as Body from R14 Onwards. Explain how this will bring additional benefit to the user. Let’s see how Geometrical Sets are managed…

Surface Design

Managing Geometrical Sets …

3

1

2

… then you will create new elements in the current Geometrical Set.

You may move the elements from a set to another.

You will first insert a new Geometrical Set…

Let ’s see now the ways to manage Geometrical Sets ...

Instructor Notes:

Give a high-level overview of the process of creating and using Geometrical Sets. Point out the reliance on Contextual Menus to Rename a Geometrical Set and Reorder elements in a Geometrical Set or move elements from one Set to another.

Let’s look at this process in more detail…

Surface Design

Inserting and Renaming a Geometrical Set Based on the licenses you have , you will sometimes not get this window. .

1 Create a new Geometrical Set. The new Set is created after the last element of the current Geometrical Set in the specification tree and is automatically set current.

2

In the properties, rename Geometrical Set into “Operations”.

Instructor Notes:

Explain the process of creating a new Geometrical Set (using the Insert menu) and how to Rename the Geometrical Set. Point out how to define a Geometrical Set in Work Object.

Let’s see how to move elements from one Set to another...

Surface Design

Moving an Element to another Geometrical Set You can move an element to another geometrical set without modifying the geometry. Select the element to be moved using mouse button 3, display its contextual menu then choose the Change Body option in the element object menu.

1

2 The Change Geometrical Set window is displayed.

In the specification tree select the destination geometrical set. To place the element precisely you can select the element above which you want to move it.

Click OK in the “change geometrical set” window.

3

The element moves to another geometrical set.

Instructor Notes:

Explain the process of using the « Change Geometrical Set » contextual menu to move an element from a set to another. Note that mult-selected elements can also be moved in one step using the Selected Objects contextual menu. Point out that since Wireframe and Surface elements do not have Order of Operation results in a Body as is the case with Solid features in Part Bodies, moving a feature from a set to another will not change the design.

Let’s see the effect of moving elements within the same Geometrical Set...

Surface Design

Moving an Element within a Geometrical Set You can move an element to another location within a geometrical set without modifying the geometry.

1

Select the element to be moved using mouse button 3, display its contextual menu then choose the Change geometrical set option in the element object menu.

In the specification tree select the element above which you want to locate it, here Sketch.2.

2

3

The “Change geometrical set” window is displayed.

Click OK in the “change geometrical set” window. The element moved before the sketch 2.

Instructor Notes:

Explain the process of reordering a feature while keeping it in the same Geometrical Set. Note that the Change Body contextual menu is used to do this even though there is no intent to move the feature to a different Geometrical set. Emphasize that Wireframe and Surface geometry does not require an Order of Operations in the Geometrical set tree.

Let’s sum up what we’ve learned about Common Tools...

Surface Design

To Sum Up ...

You have seen CATIA V5 – Shape Design Common Tools:

Stacking Commands: You have seen how this feature allows you to create input elements on the fly improving your efficiency and also reducing the size of tree. Managing Geometrical Sets: You have seen how this container can help you in managing your features in the tree.

Instructor Notes:

Point out that you have learned about three important tools in this section. These tools provide substantial capability to improve efficiency when creating or modifying Wireframe and Surface designs.

Surface Design

Creating Surfaces You will become familiar with the creation of basic surfaces

Why Create Surface Geometry ? Creating Basic Surfaces Creating a Swept Surface Creating a Surface Offset from a Reference Creating a Surface from Boundaries Creating a Multi-Section Surface Creating Basic Surfaces: Recap Exercises Additional Reference Material To Sum Up

Instructor Notes:

Surface Design

Why create Surface geometry ? For certain designs, the geometry can not be completely defined using the tools in the Part Design workbench. Complex 3D shapes often need to be defined using surface geometry which is created based on explicit wireframe construction geometry. Surface geometry can then be integrated into the final solid part definition. If the industrial context does not require a solid, surfaces are kept as it is. Key Points

Surface geometry can describe a more complex 3D shape. A surface element describes shape, therefore it has no thickness.

Surface geometry can be completely integrated into the solid part meaning surface modifications are reflected in the solid.

Surface geometry

Solid geometry

Instructor Notes:

Emphasize the Key Points on this slide to the students. Fairly complex geometries can be accomplished using Surface features.Many downstream applications use surface geometry as inputs, for example air flow analysis over a car or an aeroplane will need the skin geometry of the car.Surface geometries can be used in Structural Analysis of CATIA by giving shell property to the surface. Surfaces can be directly taken as input geometries in the machining workbench for example machining of turbine blades. Surface Geometry can be used to create Solid features, this can be the most efficient way to approach the design of certain categories of solid parts.

Surface Design

Creating Basic Surfaces

In this section you will find out about some of the easiest ways to create surfaces.

Instructor Notes:

Surface Design

The extruded surface is created from an open or closed profile, giving a direction and limits.

Cylindrical surface is created by defining a point, direction and length of the cylinder.

Instructor Notes:

A surface of revolution is created from an open or closed profile, giving an axis of revolution and an angle.

Spherical surface is created by defining the centre point, radius and an angle(in case a partial sphere is required) .

Surface Design

Creating an Extruded Surface

1

2

Select a profile, a direction and enter limits value (or use the graphic manipulators).

Using contextual menu, direction can be specified by a line, a plane or components.

Limits

Instructor Notes:

3 Click OK to confirm extruded surface creation.

Surface Design

Creating a Surface of Revolution

1

2

Select a profile, an axis of revolution and key in the angle limits.

Profile

Instructor Notes:

Axis of revolution

3

Click OK to confirm surface creation.

Surface Design

Creating a Spherical Surface 1

2

Select the sphere center point and key in the sphere radius.

3

Choose to create a complete sphere or a partial sphere.

Complete Sphere

Instructor Notes:

You can modify the partial sphere parameters in the Sphere Surface dialog box or dragging and dropping the arrows on geometry.

Partial Sphere

Surface Design

Creating a Cylinder Surface

1

Select the centre point for the cylinder:

2

5

Select a direction for the cylinder’s axis:

3

Instructor Notes:

Surface Design

Creating a Swept Surface

You will learn how to create an explicit-type swept surface

Instructor Notes:

Surface Design

Creating an Explicit-type Swept Surface 1

Select the Sweep Surface icon.

2

Select the guide curve and the profile. You can then choose to specify a reference plane or surface (Reference tab) or select another guide curve and anchor points (Second Guide tab).

By default, the swept profile is constant in each section along the guide curve. Copyright DASSAULT SYSTEMES

If no spine is selected the guide curve is used as spine.

3

Confirm swept surface creation.

Instructor Notes:

Provide an illustration by drawing on the board.

Point out how implicit reference Planes are established based on the Profile and Guide curve. Also point out how the Default Spine is derived.

Surface Design

Creating a Swept Surface - Reference Surface option

You can define a reference surface to control the position of the profile along the sweep.

You can define an angle between the profile and the reference surface

Instructor Notes:

Provide an illustration by drawing on the board. Explain the role of the Reference Surface in controlling the orientation of the Profile as it is swept.

Surface Design

Creating a Swept Surface – Second Guide and Anchor Points (1/2) You can also select a second guide curve to define the sweep.

In this case, no reference surface is needed

• If you check the Profile extremities inverted option, the profile extremities connected to the guides are inverted. • If you check the Vertical orientation inverted option, the vertical orientation of the profile is inverted.

Instructor Notes:

Point out how the anchor points drive the profile position.

Surface Design

Creating a Swept Surface – Second Guide and Anchor Points (2/2) You also can use Anchor Points to position the profile on the guide curves.

Guide curves

Profile

Anchor points

Instructor Notes:

While creating the swept surface, the anchor points lie on the guide curves from the beginning to the end of the sweep.

So, the profile is positioned in regards to the initial geometric conditions between the profile and the anchor points.

Surface Design

Creating a Swept Surface - Position Profile options (1/3) You can position the profile with the guide curve.

Using no positioning : When the profile position is fixed with respect to the guide curve, the sweep lies on the profile and on the guide curve (if it intersects the profile) or on the parallel to the guide curve crossing the profile (minimum distance). Using positioning : The profile is oriented in the guide curve axis system.

The guide curve axis system is now oriented based on the reference surface orientation :

Grey axis-system : profile reference axis

Using positioning and a reference surface :

Green axis-system : current profile orientation

Instructor Notes:

Explain the behavior of Sweeping when the Profile and the Guide Curve do not intersect.

Surface Design

Creating a Swept Surface - Position Profile options (2/3) In the Position profile mode you can display parameters to modify the position of the sweep profile on the guide curve defining a new origin and a rotation angle or direction.

Or

These coordinates (or the selected point) define the position of the origin of the positioning axis system (green) in the first sweep plane.

45 deg

You can rotate the positioning axis system around the guide curve with respect to initial axis system of the profile.

The direction defines the X axis of the positioning axis system.

Instructor Notes:

Discuss the role of origin co-ordinates and origin selection in controlling the location of the positioning axis system on the first sweep plane.

Surface Design

Creating a Swept Surface - Position Profile options (3/3) In the Position profile mode you can modify the position of the sweep profile on the guide curve by inverting an axis or selecting a point on the profile.

You may want to invert the orientation of the X or Y axes of the positioning axis system.

You can select a point defining the origin of the axis system linked to the profile.

Instructor Notes:

Point out the use of Inverted Axis Options to furthur control the Explicit Sweep.

Surface Design

Creating a Swept Surface - Spine You can impose a spine to further define the sweep.

If no spine is selected, the first guide curve is the spine :

You can select a spine if you want to obtain a more regular surface :

Instructor Notes:

Explain the difference between the Default Spine (derived from the first Guide Curve) and a Spine defined from another element. Point out the ability to use a contextual menu to define the Spine.

Surface Design

Creating a Surface Offset from a Reference You will learn how to create an offset surface.

Repeat

Instructor Notes:

Single

Surface Design

Creating an Offset Surface (1/2)

1 2

Select the reference surface and key in the offset value. Reference surface

3 If you want to create several surfaces

separated by the same offset check the option Repeat object after OK.

Object surface

4

Click OK to continue. The created offset surface is defined as an Object, i.e. the reference for creating the other surfaces.

Reference surface

Instructor Notes:

Explain that a variety of surfaces (Sweep, Revolute, etc.) can be used as reference surfaces for offsetting. Only a single surface can be referenced for creating the Offset surface, but multiple surfaces can be combined through Operations (Join, Trim, etc.) ahead of time and then offset. A single Offset surface can be created or two Offset surfaces (one in each direction) can be derived using the Both Sides option. The Repeat Object after OK option will allow for several more Offset surfaces to be created. The resultant Offset surfaces are distinct Objects that are linked to the Parent reference surface.

Surface Design

Creating an Offset Surface (2/2)

5 Define the number of offset surfaces to be created.

The surface instances are grouped in a new Geometrical set (unless you uncheck the option).

6 Click OK to confirm surface creation. Object surface

Surface instances in Geometrical Set

• As many offset surfaces as indicated in the Object Repetition dialog box are created, in addition to the object surface. • The surfaces are separated from the object surface by a multiple of the offset value.

Instructor Notes:

Explain the option under Object Repetition to create the additional Offset surfaces in a New Geometrical Set. Note that if this option is exercised, the Offset surfaces in the new Geometrical Set are still linked to the parent Surface regardless of the Geometrical Set it is in. The original Offset surface (from the previous dialogue box) will be created under the currently active Geometrical Set, but can be reordered to any other Geometrical Set after creation.

Surface Design

Creating a Surface from Boundaries

You will learn about the types of surfaces created from boundaries.

Instructor Notes:

Surface Design

Creating a Fill Surface (1/2) 1

2 Select the boundaries of the fill surface and, if needed, the support(s) associated with one or more boundary(ies).

Support for B1 B4

B2 B1 B3

Support for B3

The result of the selections must be a closed boundary.CATIA takes care of small openings upto 0.1 mm in the closed wireframe. This is tolerant nature of CATIA .

During or after creation you can edit a fill surface, adding, replacing or removing a boundary or a support. The type of continuity between the support surface(s) and the fill surface can be chosen from the Continuity combo.

Instructor Notes:

Explain that the curves used to define the Fill surface must result in a closed boundary. As a curve is selected, its support (optional) can be added by selection. When supports are added, the Continuity between the new Fill surface and those supports can be specified through a drop-down box. Options for Continuity are: Point, Tangent or Curvature. At any time during creation (or later on through modification) curves can be added, removed or replaced from the Fill surface definition. Supports can also be added, removed or replaced at any time.

Surface Design

Creating a Fill Surface (2/2) 3 You can also define a point through which the surface will pass.

The result depends on the selected type of continuity (Tangent or Point) between the support surfaces and the fill surface.

Point continuity

Tangency continuity

If you do not select any support or passing point the fill surface is simply created between the boundaries.

4 Confirm fill surface creation.

Instructor Notes:

Explain that a Passing Point will cause the Fill surface to include the point in its mapping definition so that the surface obviously will pass through the point. The effect of this passing point on the new Fill surface is also related to the type of Continuity specified for any Supports included in the definition. Fill surface provides a great way to generate surfaces between the edges of adjacent surfaces as long as the resultant boundary formed by the edges is closed.

Surface Design

Creating a Blend Surface (1/4) 1

2

Select the two curves between which you will create the blend surface and, if needed, the support associated with each curve.

The two selected curves have to be single edge curves.

Instructor Notes:

The two curves used to create a Blend surface can be open or closed. They can also be discontinuous from each other, or continuous at one point. These options provide a distinct difference from those available for Fill surfaces. Blend surfaces allow for the definition of supports for the two defining curves, including continuity definition and options to create trim the resultant blend into a single surface that incorporates its supporting surfaces.

Surface Design

Creating a Blend Surface (2/4) 3 If you have selected one or more support surface(s) define the type of continuity

(Tangency, Curvature or Point) between each support surface and the blend surface.

You can use the combo to define a different type of continuity on each side of the blend surface.

You can choose to trim the support to expand the blend surface up to the limits of the support.

Curvature continuity

Point continuity

Tangency continuity

Instructor Notes:

Explain the options for establishing continuity (Point, Tangency and Curvature) with emphasis that different Continuity types can be established on either side of the Blend surface. Describe how the Trim Support option will extend the resultant Blend surface out to include the entire extent of the Support. This is very similar to the Trim operation except that the result is still a Blend surface object.

Surface Design

Creating a Blend Surface (3/4) 4 If you have selected one or more support surface(s) you can choose to make the borders of the blend surface tangent to the borders of the supports.

For each border of the blend surface you can choose the extremity(ies) that will be tangent to the corresponding border of the support.

2nd border, end

Second support

der

bor

First bo

rder

ond Sec

1st border, start

First support First tangent border : None Second tangent border : None

First tangent border : Both extremities Second tangent border : Both extremities

First tangent border : Start extremity Second tangent border : End extremity

Instructor Notes:

Tangent Borders allows even finer control over the tangencies that are imposed on the Blend surface. Borders are implicity defined based on the Curves selected and their Supports. Instead of applying a global tangency continuity between the Blend surface and its supports, you can specify that the Tangency be selectively imposed for each resultant border. This gives much more flexibility to the user in controlling the Blend surface definition.

Surface Design

Creating a Blend Surface (4/4)

5 Select the Tension tab to define the tension at the limits of the blend surface.

You can keep the default tension or define a constant or linear tension at each limit of the blend surface.

Constant tension of 2.5

Linear tension from 1 to 2.5

Default tension

Instructor Notes:

Explain how Tension can impose Tangency incursion further into the Blend surface. Using Constant Tension, this imposition is factored contantly along the limits of the first or second curve. Using Linear Tension, this imposition can be varied with differing tensions at each end of the curve. Closing Points and Couplings provide additional means of controlling the definition of a Blend surface, but we will look at their roles in the context of a Lofted surface in the next session.

Entertain questions from the students.

Surface Design

Creating a Multi-Section Surface You will learn how to create multi-section surfaces.

Tangency

Closing point

Guide curve

Spine Coupling

Manual coupling

Instructor Notes:

Lofting uses multiple profiles (curves, boundaries, sketches, etc.) to produce a surface.

Discuss Tangencies,Closing points,Guide curves,Couplings and spines may be used to control the loft surface through the profiles.

Surface Design

Creating a Multi-Section Surface – Tangent Option For the start and end sections of the multi-section surface you can define a surface (containing the corresponding section curve) to which the lofted surface will be tangent.

Section 2

Extrude 1

Extrude 2

Section 1 No tangency condition is imposed between the multi-section surface and the two extruded surfaces.

The multi-section surface is tangent to the two extruded surfaces.

Instructor Notes:

Tangent option provides a means to impose a tangency from either end (or both ends or neither end) of the Lofted surface to an adjacent surface.

Surface Design

Creating a Multi-Section Surface - Closing Points (1/3) When you create a multi-section surface from closed sections a closing point can be defined for each section. The closing points are linked to each other to define the multi-section surface orientation. You can also change the closing point of one or more section(s) to modify the multi-section surface orientation. User defined closing points

Default closing points defined

The closing points are linked to each other.

Instructor Notes:

Demonstrate the concept to the students. Explain to the students that Closing Points provide a mean of orienting how the surface is Lofted between the Sections. Inconsistencies and geometric errors can result from Closing Point definitions on different Sections that lead to a Cusp in the Multi-section surface mapping.

Surface Design

Creating a Multi-Section Surface - Closing Points (2/3)

To create the multi-section surface you will select and orient the sections then define the closing point for each of them.

To define a closing point on a section, select the section then click on the adequate point. The point is mentioned in the Closing Point list in front of the corresponding section.

Instructor Notes:

Surface Design

Creating a Multi-Section Surface - Closing Points (3/3) Changing a closing point on a section

1

Select the sections.

For each section the starting point of the arrow defines the default closing point.

Instructor Notes:

2

Right click on the default closing point and select “Replace”:

3

Select a point on the section to define the new closing point:

Surface Design

Creating a Multi-Section Surface – Guide Curve To define the evolution of the multi-section surface between two consecutive sections you can select one or more guide curve(s). The guide curve(s) must intersect the two sections of the multisection surface. Section 2

Section 1 Without Guide Curve

Guide curve 2

Guide curve 1

With Two Guide Curves

Instructor Notes:

Demonstrate the concept to the students

Surface Design

Creating a Multi-Section Surface – Spine The spine guides the section orientation. You can either keep the default spine (automatically computed) or choose a user-defined spine selecting a line or a curve.

Section 1

Section 2

Spine

With a Computed Spine

With a User-Defined Spine

Instructor Notes:

Important Topic: Explain that a spine guides the orientation of a Lofted surface. CATIA computes a default Spine through the selected Sections. The Section orientation can also be guided along a user-defined Spine (Line, Curve or Spine from the GSD workbench). Note that if a user-defined Spine is specified, the Spine curve must be continuous in tangency.

Surface Design

Creating a Multi-Section Surface - Coupling (1/6) The coupling tab in the multi-section surface function is used to compute the multisection surface using the total length of the sections (ratio), between the vertices of the sections, between the curvature discontinuity points of the sections or between the tangency discontinuity points of the sections. Vertices, Curvature Discontinuity, Tangency Discontinuity Ratio option

Vertices, Curvature Discontinuity

Curvature discontinuities option

Vertex

Instructor Notes:

Couplings are of two basic configurations: Curvilinear Abcissa- a Coupling between 2 consecutive sections. By Spine- a Coupling controlled by the Guides definition in the Lofted surface. When creating Couplings through Sections, different Coupling Types are available (depending on the geometric configuration of the Sections): Ratio Tangency Tangency then Curvature Vertices

Surface Design

Creating a Multi-Section Surface – Coupling (2/6)

What types of points can CATIA use to split the sections when creating a multi-section surface using coupling ?

These two points are tangency and curvature discontinuity points. They are also vertices.

To have a look at the different discontinuities, we have sketched a profile as shown below :

Segments

Two arcs

These two points are curvature discontinuity points. They are also vertices.

This point is a tangency and curvature continuity point. This point is a pure vertex.

Instructor Notes:

The Sections used to create the Lofted surface are split through point definitions along the Section profile. These points may have attributes of being a pure vertex or vertices with tangency and/or curvature continuity. How these points are categorized plays a result in how the Lofted surface is generated when different Coupling Types are applied.

Surface Design

Creating a Multi-Section Surface – Coupling (3/6) Ratio-type coupling :

to compute the multi-section surface using the total length of the sections

The surface crosses the sections and the variation between the sections is computed by a ratio corresponding to the length of each section.

Instructor Notes:

When the Ratio type of Coupling is applied, the computation of the Isoparameters is performed using the curvilinear abcissa ratio computed between the Sections. In more complex Lofted surface definitions, the Ratio type of Coupling does not often produce a desirable set of Isoparameters for the Lofted surface. You may wish to point out to the students how the additional edges are created on the upper portion of this example to show this type of problem with Ratio Coupling.

Surface Design

Creating a Multi-Section Surface – Coupling (4/6) Tangency-type coupling :

to compute the multi-section surface between the tangency discontinuity points of the sections

The surface crosses the sections and each section is split at each tangency discontinuity point. The surface is computed between each split section.

Instructor Notes:

When Tangency type Coupling is applied, the Sections are split and the Loft is computed from each point on the Section where a Tangency Discontinuity exists. It is important to note that the curves on each Section must have the same number of Tangency Discontinuity points or this option cannot be used for Coupling. Point out to the students that our example now has a more acceptable Isoparameterization on the upper portion of the Lofted surface, but this option does not correct the extra faces created on the bottom portion.

Surface Design

Creating a Multi-Section Surface – Coupling (5/6) Tangency then Curvature-type coupling :

to compute the multi-section surface between the curvature discontinuity points of the sections

The surface crosses the sections and each section is split at each curvature discontinuity point. The surface is computed between each split section.

Instructor Notes:

When Tangency then Curvature type Coupling is applied, the Sections are split and the Loft is computed according to their Tangency Continuity first and then their Curvature Discontinuity points next. Once again, the same number of points must exist on each Section. Point out to the students that our example now has a more acceptable Isoparameterization all around.

Surface Design

Creating a Multi-Section Surface – Coupling (6/6) Vertices-type coupling :

to compute the multi-section surface between the vertices of the sections

The surface crosses the sections and each section is split at each vertex. The surface is computed between each split section.

Instructor Notes:

When Vertices type Coupling is applied, the Sections are split and the Loft is computed according to Vertices of each Section. Once again, the same number of Vertices must exist on each Section.

Surface Design

Creating a Multi-Section Surface – Manual Coupling (1/3) When the sections of the Multi-Section surface do not have the same number of vertices you need to define a manual coupling.

1

Define the sections and guide curves if needed.

2

Select the Coupling tab from the MultiSection Surface Definition window.

Double-click in the blue Coupling field to display the Coupling window.

3

Instructor Notes:

Reemphasize to the students that when the Sections used for defining a Multi-Section surface do not have the same number of points, only the Ratio type of Coupling is available for automatic creation of the Multi-Section. However, it is possible to manually create Couplings between Sections that do not have the same number of points. This is done by activating the Coupling tab and then selecting two points (one on each Section) that will be used to create the manual Coupling. As many manual Couplings as necessary to derive the desired Multi-Section can be created.

Surface Design

Creating a Multi-Section Surface – Manual Coupling (2/3)

4

For each section select the vertex to be taken into account in the coupling then click OK to end coupling definition. You can visualize the coupling curve if the corresponding option is checked.

5

To refine the shape of the lofted surface you can define another coupling curve : select the first coupling and click on the Add button, then define the new coupling curve as explained above.

6

Click OK to end Multi-Section surface definition. At any time you can edit a coupling by double-clicking on the coupling name in the list and changing the coupling points using the contextual menu.

Instructor Notes:

Point out to the students how two Manual Couplings have been created in this example, each Coupling sharing a single Vertex on Section 2. Couplings can be visualized by checking that option in the dialogue box, but actual curve elements are not created.

Surface Design

Creating a Multi-Section Surface – Manual Coupling (3/3) You will find below various cases of manual coupling with one or more coupling curves. One coupling curve (2)

Two coupling curves

One coupling curve (1)

Instructor Notes:

You can show the students various results from different Manual Couplings.

Surface Design

Creating Basic Surfaces Recap Exercises 25 min

You will now do the following exercises Button Mouse

Instructor Notes:

Surface Design

Creating Basic Surfaces Recap Exercise: Button 5 min

In this recap exercise you will create : Use Wireframe geometry completed in previous exercise to create Surface geometry that will be used to shape the solid part. Extrude with Plane as direction Extrude with Line as direction

Instructor Notes:

Surface Design

Creating Basic Surfaces Recap Exercise: Mouse 15 min

In this recap exercise you will create : A swept surface for the top shape of the mouse Two extruded surfaces to shape the side and front of the part A blend surface to connect existing surfaces while maintaining tangency

Instructor Notes:

Surface Design

Additional Reference Material Additional information can be found in the following reference material: Companion: Skillets: Creating a Surface from a profile, creating a spherical surface,

creating a cylinder surface, creating a swept surface, creating a surface offset from a reference, creating a surface from boundaries, creating a multi-section surface

Keywords: sweep, surface, extrude, sphere, loft, multi, section, offset, blend, cylinder, revolve

Books:

Mechanical Design Solution – Wireframe & Surface Design Shape Design Solution – Generative Shape Design

Search String:

Extrude, Revolve, Sphere, Offset, Sweep, Fill, Blend, Loft, Coupling, Spine

Instructor Notes:

Present the different Companion documents available for additional information and the on-line documents. NOTE: a demonstration is preferred to assist the students in locating the documents and showing at least one of them. It should be state that these sources of documentation do a good job in covering the features.

Surface Design

To Sum Up ...

You have seen CATIA V5 – Creating Basic Surfaces:

How to create surfaces from a profile using Extrude command and Revolve command. How to create a spherical surface using the Sphere command. How to create a cylinder surface using the Cylinder command. How to create a swept surface using the Sweep command. How to create surfaces offset from a reference using the Offset command. How to create surfaces from boundaries using the boundary or the extract command. How to create multi-section surfaces.

Instructor Notes:

Surface Design

Performing Operations on the Geometry

You will learn how to perform operations on the geometry

Why are Operations on Geometry needed ? Joining Elements Splitting/Trimming Creating Fillets Transforming Elements Extrapolating Elements Disassembling Elements Additional Methods for Operations Operations on Geometry: Recap Exercises Additional Reference Material To Sum Up

Instructor Notes:

Surface Design

Why are Operations on Geometry needed ? (1/2) After the basic surface geometry is created, it may be composed of construction elements that do not describe the finished shape. Operations such as trim, join, extrapolate, and transform are then performed to produce the required finished geometry.

Operations are used to produce the finished geometry shape.

Key Points

Elements involved in an operation are kept in the history of the operation but placed in hide.

Healing is an important capability that can be used to repair the gaps that exist in surface geometry.

Surface fillet operation

Instructor Notes:

Healing Operation

Surface Design

Why are Operations on Geometry needed ? (2/2) Transformations like scaling and affinity help in resizing up the part if required. Transformation operations like translate and rotate are required on the wireframe elements (lines and planes) to change the positioning of the part in the co-ordinate axis system. Key Points

Affinity is an important operation to resize the part differently in different directions according to a defined axis.

Axis to Axis transformation is useful when we want to have more than one reference axis systems and part elements are required to be moved from one axis to other.

Affinity Operation.

Instructor Notes:

Axis to Axis transformation.

Surface Design

Joining Elements You will learn how to join wireframe or surface elements.

Element 2

Element 1

Instructor Notes:

Join result

Surface Design

Why Do You Need Joining Elements ? You can join elements to use two or more elements as a single element in a further operation.

What about joined elements ? You can create joined elements from: - adjacent curves - adjacent surfaces

Join result

Join result

Instructor Notes:

Explain to the students what Joining Elements are and why they might want to create them. Joining Elements can be created from two or more adjacent curves. Joining Elements can be created from two or more adjacent surfaces. The resulting single element from the Join can be used to create additional elements. The Join is associative with the elements used to create it.

Surface Design

Joining Elements (1/2) 1 2

Select one by one the elements to be joined together. Element 1

Element 2

This option checks the connexity between the elements in the resulting join.

To modify the join definition you can edit it and remove elements or replace an element by another.

CATIA will: - reduce the number of resulting elements - ignore the elements that do not allow the join to be created.

You can define a merging distance, i.e. the maximum distance below which two elements are considered as only one element.

3

Click OK to confirm join operation.

Instructor Notes:

Explain that elements have to be adjacent in order to be joined only when the Check Connexity box is checked. If this box is not checked, then large gaps can exist between elements and they can still be Joined. When the Check Connexity box is checked, there can be no gaps in adjacent elements that have a value above that specified in the Merging Distance field of the dialogue box. The Merging Distance value must be less than 0.1mm. Explain the purpose of Result Simplificiation.

Surface Design

Joining Elements (2/2) While joining elements you can exclude some sub-element from the joined surface.

You can also select sub-elements to exclude from the joined surfaces.

Face to be removed

You can create another join surface with the excluded sub-elements.

Instructor Notes:

Explain what sub-elements are (faces, etc.) and why you might want to remove them from a Join. Point out that the sub-elements that are removed from the Join can be used to create a separate Join by checking the option in the dialogue box. The example here uses surfaces, but these options also apply to wireframe elements.

Surface Design

Splitting/Trimming You will become familiar with Splitting and Trimming elements

Splitting Elements Trimming Elements

Instructor Notes:

Surface Design

Splitting Elements You will learn how to split a wireframe or surface element using one or more cutting elements

Cutting elements

Split result

Element to be cut

Instructor Notes:

Surface Design

Why Do You Need Splitting Elements ? You can split an element when you need only part of this element in your model. You need the element to be cut and one or more cutting element(s).

You can split : a wireframe element by points, other wireframe elements or surfaces a surface by wireframe elements or other surfaces. Cutting elements

Element to cut

Cutting element

Element to be cut

Wireframe elements

Surface elements

Split result

Split result

Instructor Notes:

Explain to the students they might wish to create a Split. Splits are useful in developing more complex geometry from more basic shapes. Point out to them that the resultant Split remains associative to the original element to cut and the cutting element(s). Discuss the different types of Splitting Elements that can be used, depending on the type of geometry being cut.

Surface Design

Splitting Elements (1/2) 1 2

Select the element(s) to cut. Select the cutting element(s).

3

You can split one or more elements with one or more cutting elements at the same time.

Cutting elements

If you select only one cutting element you can check this option to keep the two sides of the element to cut. In that case two split features are created.

You can create the intersection between the cut element and the cutting elements. If this button is selected, the features are automatically extrapolated so that the operation can be processed.

Elements to cut A surface can be split using a plane, a surface or a line. The line has to lie on the surface you want to split.

Instructor Notes:

Explain to the students the options available in the dialogue box. Make note of the additional option when only one Cutting Element is defined and the purpose of an Intersection Computation. Clearly explain to students about the ability to select multiple elements in the element to cut. Also mention the limitation.

Surface Design

Splitting Elements (2/2)

4

For each selected cutting element check the side to be kept on the element to cut; if you want to change it select the cutting element in the list and click on the Other side button. The cutting

elements and their orientation are defined.

Click OK to confirm the split operation.

5

Instructor Notes:

The initial cut element is transferred to the ‘hide’ space.

Surface Design

Trimming Elements You will learn how to trim wireframe or surface elements.

Element 1

Instructor Notes:

Element 2

Trim result

Surface Design

Why Do You Need Trimming Elements ? You can trim elements between each other to only keep part of them. You need intersecting elements to perform Trim Operation.

What about trimming elements ? You can trim : Multiple wireframe elements (Pieces Option), Multiple surfaces and wireframe (Standard Option).

Trim result Wireframe elements

Instructor Notes:

Surface elements

Trim result

Surface Design

Trimming Elements… Trim operation for wires can be done using “Pieces” option or “Standard Option” Using ‘Standard’ option you can trim multiple elements (both surfaces and wireframe) at a time. For example the trim result of first two elements is given to the third element.

‘Pieces’ option can be used to trim multiple wires that are intersecting. The selection can be sequence independent. 3

1

2

4

5

7

6

Selection: 1-3-4-7

Instructor Notes:

Explain that the same methodologies that the students used to create Splits also apply to Trimming. Point out the technique of selecting the side to keep.

Surface Design

Trimming Elements using ‘Standard’ Option. ‘Standard’ option can be used for trimming multiple surface/wire at the same time. 1 2 3

Select two surfaces to trim (A and B).

A 4

Orient the result of the previous selection and select the third surface (C).

The result of trim for the first two inputs is sent as an input for trimming with the third element.

5

Confirm OK.

Instructor Notes:

B

Select the standard Option.

A B c

c

You can use ‘Element to keep’ or ‘Element to remove’ options to refine the result you need.

Surface Design

Creating Fillets

Filleting is an operation that is used to smoothly connect surfaces. You will learn how to create Shape, Edge, Variable, Face-To-Face, and TriTangent Fillets.

Instructor Notes:

Explain that just as there is sometimes a requirement in Part Design (using solid features) to make smooth transitions between faces that share an edge, there can also be a requirement to smoothly blend two or more surfaces together along contiguous edges.

Surface Design

Why Fillets? Fillets were originally used in industry to remove sharp edges on parts. Fillets along with drafts help in the easy removal of material from molds. Fillets also help in reducing stress concentration in parts.

More and more, people having been using Fillets as a general modelling tool for surface creation.

Let ’s see how to create fillets ...

Instructor Notes:

Explain that Fillets originated as a manufacturing method to break sharp edges on parts. With the advent of a wide range of 3D modelling tools in CAD systems, designers are using Fillets to develop part designs and not just to support manufacturing processes. Fillets are under the Part Design Shared Package in the Catia Object Library. The process of creating Fillets is identical between Part Design and Wireframe and Surface Design except that Shape Fillet is only used in Wireframe and Surface Design or GSD.

Surface Design

Creating a Shape Fillet Use this command to create a fillet between two surfaces.

1

Select the Shape Fillet Icon

Select two surfaces/faces and put in the required radius value. Make sure the red arrows point towards the concave side of the fillet.

3

Choose one of the Extremities conditions (Switch between the four types - and Preview - to see the difference)

2

4 Click OK to confirm. The Shape Fillet is added to the specification tree.

Instructor Notes:

Explain the purpose of using a Shape Fillet to create a smooth transition between two surfaces (using the BiTangent Fillet Type option) or three surfaces (using the TriTangent Fillet Type option). Point out that a Directional Arrow is displayed for each surface selected. It is important that these arrows point in a consistent direction toward the Concave side of the Fillet that is being created. The Shape Fillet will be generated based on the Radius that is keyed in and the Extremities type that is specified.

Surface Design

Creating an Edge Fillet (1/2) Use this command to provide a transitional surface along a sharp edge of a surface

3

1 Select the Edge Fillet Icon

2

You can control the Extremities of the Fillet the same way as for the Shape Fillet.

Select one or more edges of a surface

You can also fillet an entire face.

Instructor Notes:

Explain the difference between a Shape Fillet (a fillet blend between two or three separate surfaces) and an Edge Fillet (a fillet along the sharp edge or edges of a single surface). Point out that single or multiple edges, single or multiple faces, or a combination of edges and faces can be selected on the surface for filleting.

Surface Design

Creating an Edge Fillet (2/2) 4

Choose a Propagation type :

If Minimal, only the selected edges will be filleted.

If Tangency, all edges tangent to the selected edges will also be filleted.

5

Click OK to confirm. The Edge Fillet is added to the specification tree.

Don’t forget to choose “Define In Work Object” for the Geometrical Set

Instructor Notes:

Differentiate the two propogation modes.

Surface Design

Creating a Variable Radius Fillet (1/2) In this type of fillet the radius varies at selected points along a selected edge

Select the Variable Fillet Icon

1 2

Select one or more internal edges of a surface

3

Double-Click on any of the shown radius values to change it You can specify a Zero radius value at limit points of a Variable Fillet

4

Select inside this box then select anywhere along the edge to put in an additional radius value along the edge. (You can also create a point on the edge and select this point if accuracy is required) You can control the Extremities of the Fillet the same way as for the Shape Fillet and the Propagation type the same way as for the Edge Fillet

Instructor Notes:

Explain the process of defining Variable Radius Fillets on Surfaces edges. Discuss how additional Points can be added to the edge(s) by clicking the approximate location for a radius variation. Note that this method does not provide a means to precisely constrain the location of the radius variation.

Surface Design

Creating a Variable Radius Fillet (2/2) 5

Choose a radius variation type : Cubic (function ax3+bx2+cx+d)

Linear (function ax+b)

6

Click OK to confirm. The Variable Fillet is added to the specification tree.

Instructor Notes:

Point out the Forumulaic Differences between Cubic Variation and Linear Variation along the edge being filleted.

Surface Design

Creating a Face-To-Face Fillet Use the Face-Face fillet command when there is no intersection between the faces or when there are more than two sharp edges between the faces.

2

1

Select the Face-To-Face Fillet Icon

3

4

Click OK to confirm. The Face-To-Face Fillet is added to the specification tree.

Select the two faces (belonging to the same surface) between which you want to create the Face-ToFace Fillet

You can control the Extremities of the Fillet the same way as for the Shape Fillet

The shape of the Face-To-Face Fillet is basically generated by laying a Cylinder with a specific radius into the gap between two faces. If the radius is too small, the Cylinder will not be able to touch both faces at once. If the radius is two big, it will not be able to achieve a Cylinder tangent to the faces.

Instructor Notes:

Explain the dialogue box options for creating a Face-to-Face Fillet. Point out to the student that the Faces selected must belong to the same Surface. This may require the separate surfaces to be Joined prior to creating the Fillet. Also note the limitations imposed for this type of Fillet– errors can result if the faces selected do not allow a cylinder development and tangency between the Fillet and the two Faces based on the Specified Radius.

Surface Design

Transforming Elements

You will learn the various transformations you can apply to elements.

Instructor Notes:

Surface Design

Why Do You Need Transformations ? Transformations are used to modify the size, location, orientation of a wireframe or a surface element.

Rotation

Scaling

Affinity

Axis-to-Axis

Symmetry

Six transformation types are available:

Instructor Notes:

Describe each of the six Transformation methods available for use. Point out that each Transformation can be applied to single or multi-selected elements. The resultant Transformation is associative with the Parent features used to create it.

Surface Design

Applying Transformations… 1

Click on any Transformation icon.

2

For each type of transformation a dialog box is displayed.

The dialog box contents changes according to the selected type of transformation.

3

Enter transformation specifications in the dialog box and confirm.

Instructor Notes:

Explain that each Transformation type has its own dialogue box with fields to specify the element(s) being Transformed and their Transformation specifications. (Translate requires a Direction and Distance, Symmetry requires a reference plane, etc.) Note that all Transformation elements have an option to Hide or Show the element(s) being Transformed. This can be either way using the “Creation” choice. When the “Modification” choice is made, the initial feature is always hidden.

Surface Design

Rotating an Element (1/2)

1 2

Select the element to be rotated and define the rotation axis and the angle. Initial element

You can click this button to hide or show the initial element in “Creation” mode.

3

If you want to create several rotated elements check the option Repeat object after OK.

Object element

4

Click OK to continue. The created rotated element is defined as an Object, i.e. the reference for creating the other rotated elements.

Instructor Notes:

Explain the inputs for defining a Rotation.

Initial element

Surface Design

Rotating an Element (2/2) 5 Define the number of rotated elements to be created.

The element instances are grouped in a new Body (unless you uncheck the option).

6 Click OK to confirm element creation.

Object element

Element instances in Geometric set.

• As many rotated elements as indicated in the Object Repetition dialog box are created, in addition to the object element. • The rotated elements are separated from the object element by a multiple of the angle value.

Instructor Notes:

Point out the options in Object Repetition dialogue box. These are the same options previously shown with Translate.

Surface Design

Applying a Symmetry to an Element

1 2 Select the element and a point, line or plane as reference. Reference Line Transformed element

You can click this button to hide or show the initial element in “Creation” mode.

Reference plane Symmetry along plane

3

Symmetry by Line

Click OK to confirm symmetry creation.

Instructor Notes:

Explain the options for creating a Symmetry. Note that Reference element for the Symmetry can be a point (or vertex), line (or edge) or plane (or planar face). Repeat Object after OK is not available for Symmetry.

Surface Design

Extrapolating Elements You will learn how to create extrapolated curves and surfaces.

Curve extrapolation

Surface extrapolation

Instructor Notes:

Surface Design

Why Do You Need Extrapolating Elements ? You may have to extrapolate a curve or surface to extend it to other geometry and thus be able to later trim, split or intersect these elements.

You can extrapolate: any type of curve or line, any type of surface. Two extrapolation modes are available: giving a length, giving a limit (up to). You can obtain the result: extrapolated element as separate entity. extrapolated element as assembled with parent entity.

Curve elements

Instructor Notes:

Surface elements

Surface Design

Extrapolating Elements (1/2) 1 2

Select the edge representing the boundary you want to extrapolate. For a curve the boundary is one of the curve extremities. Surface boundary

3

Select the surface to be extrapolated. For a curve select the curve itself.

A temporary extrapolated surface is displayed. The default extrapolation mode is ‘Length’. Temporary extrapolated surface

Instructor Notes:

Explain the options for creating an Extrapolating element. Point out the types of Boundary elements that can be selected depending on the element being Extrapolated.

Surface Design

Extrapolating Elements (2/2) 4

Choose the extrapolation mode. - Length : key in the length of the extrapolated surface or curve, - Up to element : define the limit surface or plane.

5 Choose the type of continuity (for a curve or surface) and the type of extremities (propagation). Refer to table on next page.

6

Check the ‘Assemble result’ option if you want the extrapolated surface to be assembled to the support surface.

You can use the option of ‘Constant distance Optimization’ if you need a constant distance of extrapolation across the surface.

7

Click OK to create the extrapolated surface.

Instructor Notes:

Explain the different Types of Extrapolation that can be performed. Note the dialogue box options for each Type. Point out the Assemble Result option and what it means.

Surface Design

Disassembling Elements You will learn how to disassemble multi-cell surfaces or curves into mono-cell elements.

Thee monocell surfaces

Instructor Notes:

One multi-cell extruded surface

Surface Design

Disassembling a Surface 1

2

Select the element to be disassembled. The Disassemble window displays the number of selected elements and the number of resulting elements.

Extruded surface

3

Click OK to disassemble the surface.

The resulting surfaces are datum features : they cannot be modified.

You can also disassemble a multi-cell curve.

Instructor Notes:

Explain to the students that depending on the type of element selected, they will have the option to perform a Complete Disassembly to All Cells or Domains Only. The Domains Only option is only available when the element being Disassembled is not contiguous (i.e. a Join or Sketch that has elements within it that are not adjacent). The elements resulting from a Disassembly are Datums.

Surface Design

Additional Methods for Operations You will become familiar with some additional methods of performing Operations on elements

Healing Elements Restoring Elements Creating Elements from Surface Inverting Orientation

Instructor Notes:

Surface Design

Healing Elements You will learn how to fill gaps between surfaces

Surface 1 Gap

Surface 2

Instructor Notes:

Healing result

Surface Design

Healing Elements (1/2) 1

2

Select the surfaces to be healed. You can also select a Join that needs to be healed. Sweep.1

Gap

Sweep.2

3

Define the Merging distance. The merging distance is the maximum distance between the surfaces below which the gap will be filled.

Instructor Notes:

Explain the purpose of Healing (i.e. to fill in gaps between adjacent surfaces) and point out that Joins previously created without using Check Connexity or Tangency can also be Healed. Specifying a Merging Distance allows tolerance control over gap Healing. This option is specified for Point Continuity type of Healing. (not MD2) When Tangent Continuity Healing is specified, the tolerance for Tangecy angle can also be specified.

Surface Design

Healing Elements (2/2)

4

Define the Distance objective. The distance objective is the threshold below which the gap will be ignored by the heal operation.

5

Click OK to confirm the healing operation.

Instructor Notes:

Explain that in a Healing operation, the resultant element can still contain gaps. Gaps below the specified Distance Objective will be ignored. The maximum value for the Distance Objective is 0.1mm. (not MD2) When Tangent Continuity is specificed, non-tangent elements will be made tangent if their Tangency deviation is below that specified in the Tangency Angle field. (not MD2) The resultant Healed element can still contain non-tangencies. Tangency Deviations below the specified Tangency Objective will be ignored. The value ranges for the Tangency Objective is between 0.1 degree to 2.0 degrees.

Surface Design

Restoring Elements You will learn how to restore the limits of surfaces or curves which have been split before.

Restored surface

Split surface

Cutting elements

Instructor Notes:

Surface Design

Restoring a Surface You can rebuild the limits of a surface which has been split one or several time(s). Second split

Initial surface

First split

The surface limits will be restored from the second split.

1

2

Select the surface for which limits will be restored. The Untrim window displays the number of selected elements and the number of resulting elements. Click OK to restore the surface.

3

Second split You can also restore the limits of a curve which was split before.

Instructor Notes:

Explain that Restore is also referred to as Untrim and is used to rebuild a surface or curve that has been previously split. If the Split that is being restored is the result of several Split operations, the underlying definition of the original element to be Split will be Restored. Point out to the students that if the surface to be Restored is closed (i.e. a cylinder) or infinite (i.e. extruded) then the initial surface and the untrimmed surface may be identical.

Surface Design

Creating Elements from Surfaces You will learn how to create the boundaries of a surface and extract edges or faces from surfaces.

Boundary with limits

Instructor Notes:

Edge extraction

Face extraction

Surface Design

Creating the Boundaries of a Surface (1/2) You can create the external or internal boundaries of a surface, with or without limits.

1

2

Choose the propagation type and select the surface edge from which you want to create a boundary curve. You may also want to define limits to the created boundary curve. Limit points

Selected Edge

See next screen to display the various propagation types.

3 Click OK to confirm boundary creation.

Instructor Notes:

Explain to the students what a Boundary is (edge curve associated to a Surface) and how it might be used to support the creation of other geometry. Point out that a Boundary can also be used to generate associative wireframe curves along the edges of solid faces. The extent of the Boundary generation can be limited by Point or Vertex selections. A contextual menu is available to create points, if necessary. If the Limit Point does not lie on the Selected Edge, then Limit will be established by projecting the Limit Point onto the edge (normal to the edge curve).

Surface Design

Creating the Boundaries of a Surface (2/2)

1. Complete boundary

2. Point continuity

You will select a propagation type to create exactly the necessary portion of curve.

3. Tangent continuity

4. No propagation

Instructor Notes:

Explain the four different options for Propogation Type. Point out how the combination of Propogation Type and Limit Point definitions can provide many different end results for the Boundary. Boundaries are associative to the Surface and Limits that generate them, unless they are created as Datums.

Surface Design

Extracting an Edge from a Surface You can extract one or several edges of a surface which can be either boundaries or limiting edges of faces. You cannot define limit points.

1

2

Selected edge

Select a surface edge and choose the propagation type.

3

Click OK to confirm edge extraction.

According to the selected propagation type you get :

Here there is an ambiguity about the propagation side you are prompted to select a support face. In this case, the dialog box dynamically updates and the Support field is added.

Selected support face 1- No propagation

2- Tangent continuity

3- Point continuity

Instructor Notes:

Explain the process of creating an Extract curve from a Surface edge. Note the various options under Propogation Type. Point out that Point Continuity and Tangent Continuity may require the definition of a Support if the selected edge as more than one side around which to propogate the Extract. Extract can also be applied to the edges of Solid Features created with Part Design.

Surface Design

Extracting a Curve: G2 Continuity (1/2) You can define Threshold values to ignore small discontinuities, while extracting an edge of a surface or sub elements of a wire. 1

3

Select the Extract icon.

2

Select the part of the edge you want to extract:

Select the Propagation type “Curvature continuity”.

Curvature and Angular discontinuity values are shown at each node of the selected edge. You can make use of these values to define Threshold.

Click on ‘Show parameters’ to

4 define threshold values.

Instructor Notes:

Explain the Curvature choice. Explain how the curvature Threshold value determines whether or not the extraction continues through a certain curvature discontinuity.

Surface Design

Extracting a Curve: G2 Continuity (2/2) 5

Specify the Distance, Angular, and Curvature Threshold values.

To extract the full edge Define the Threshold values as shown in dialog box.

Click OK to confirm the extraction creation.

6

Extracted Edge

Instructor Notes:

Explain the Curvature choice. Explain how in addition to curvature threshold, distance and angular threshold value determines whether or not the extraction continues through a certain discontinuity.

Surface Design

Extracting a Face from a Surface You can extract one or several faces of a surface with or without propagation.

1

2

Select a face and choose the propagation type.

3

Selected face

Click OK to confirm face extraction.

According to the selected propagation type you get :

1- No propagation

2- Point continuity

The initial and the extracted faces are superimposed.

3- Tangent continuity

Instructor Notes:

Note the Propogation Type and its effect on the resultant Extract. Point out that the Extract can be derived from mutiple elements. Once more than one element is selected to create the Extract, a contextual menu and an icon become available to manage the element list. Also explain the use of the Complementary Mode to reverse the current element selection in order to create the Extract from the complementary elements.

Surface Design

Inverting Orientation You will learn how to invert the orientation of Curves and Surfaces.

Inverting a Surface

Inverting a Curve

Instructor Notes:

Surface Design

Why Invert Orientation?

The results of most surface creation and trimming operations depend on the orientations of the elements involved. Most menu interfaces allow the user to change these orientations on the fly.

The Invert Orientation operation helps while using some advanced options like Powercopy

Instructor Notes:

Explain why you might wish to create an Inverse element. Point how many wireframe and surface elements have options to specify a Negative Distance for the resultant element. Discuss options for driving the new elements through formula and how such relationships require the accomodation of the Negative Distance. Explain how deriving the child element from an Inverse will allow the relationships to utilize a Positive Direction. Point out that many elements allow you to Invert Orientation on the fly, using the Reverse Direction button. Applying this option does not create a new feature. The Invert Orientation feature exists only for your convenience where you need to change the implicit orientation of an element and create a related element with those properties.

Surface Design

How to Invert Orientation

1

Access the Invert Orientation from the Menubar - under Insert/Operations.

2

Select the curve or surface to invert its orientation. The initial display of the red arrow is the already inverted direction.

3

4

Clicking on the red arrow or on the Reset Initial button displays the initial (uninverted) orientation of the element.

Click OK to confirm. The Invert operation is added to the specification tree.

Instructor Notes:

Point out that Invert Orientation is available through the Insert toolbar and not as a Workbench tool. Explain the process of creating the Invert and note it maps exactly to the source Element and is linked to it. The only difference between the Invert and the source Element is the Inverted Orientation.

Surface Design

Operations on Geometry Recap Exercises 40 min

Mouse (operations)

Torch

Instructor Notes:

Surface Design

Operations on Geometry Recap Exercise: Mouse 10 min

In this recap exercise you will: Create more refined Surface geometry for the shape of the mouse Organize the surface geometry in the tree using a new Geometrical Set Extrapolate a surface to cover the entire Side surface for the Mouse Apply a Surface Fillet Create a Join Finally, Trim the surfaces to Create a Surface of a Mouse

Instructor Notes:

Surface Design

Performing Operations on Geometry Recap Exercise: Torch 30 min

In this recap exercise you will: Create a Join surface Split and Trim Surfaces Heal a surface

Instructor Notes:

Surface Design

Additional Reference Material Additional information can be found in the following reference material: Companion: Skillets: Creating Datum Features, Manipulating Elements Keywords: Datum, Manipulate Documentation: Books:

Mechanical Design Solution – Wireframe & Surface Design Shape Design Solution – Generative Shape Design

Search String:

Join, Healing, Trim, Split, Fillet, Extract, Untrim, Orientation, Near, Tangent

Instructor Notes:

Present the different Companion documents available for additional information and the on-line documents. NOTE: a demonstration is preferred to assist the students in locating the documents and showing at least one of them. It should be state that these sources of documentation do a go job in covering the features.

Surface Design

To Sum Up ... You have seen CATIA V5 performing operations on geometry:

How to join elements(Create a single feature in the tree by joining adjacent surfaces or wireframe) How to disassemble elements How to split elements and trim them How to create fillets using different commands like Shape fillet, Edge fillet, Variable Radius fillet, Face-Face fillet How to extrapolate elements How to transform elements How to heal elements(To fill small gaps between surfaces automatically) How to restore the limits of elements How to create elements from surfaces How to invert element orientation How to create near elements

Instructor Notes:

Surface Design

Completing the Geometry in Part Design You will learn how to complete the surface geometry in Part Design

Why Complete the Geometry in Part Design ? Creating a Solid from Surfaces Completing Geometry Recommendations Completing the Geometry in Part Design: Recap Exercises Additional Reference Material To Sum Up

Instructor Notes:

Surface Design

Why Complete the Geometry in Part Design ? In order to produce our design as a solid model, we use the Part Design workbench to integrate surface geometry into a solid part. The hybrid modeling capability of V5 allows the complex surface geometry to shape the solid part.

Key Points

The Part Design workbench is used to produce solid geometry based on complex surfaces.

Modifications to the surface geometry are reflected in the solid part.

Surface geometry

Instructor Notes:

Solid Created from Surface

Solid geometry

Surface Design

Creating a Solid from Surfaces

You will learn how to create a solid from surfaces.

Instructor Notes:

Surface Design

Why Do You Need to Create a Solid from Surfaces ? You may need to create a surface just for using it in a solid body. The surface is integrated into the body design.

What about solids created from surfaces ?

You can use a surface to: split a solid body create a solid body by thickening the surface close it into a solid body

Split Body

Instructor Notes:

Thicken Surface

Close Surface

Surface Design

Splitting a Body with a Surface 1

2 Select the surface used as splitting element and orient the arrow towards the material to be kept. Material to be kept

Splitting surface

3 Click OK to split the body.

Instructor Notes:

Explain the process of Splitting a Solid Body with a Surface. Point out that a Split solid feature is created in the Active Part Body when this operation is performed. All Solid Features in the Active Part Body tree prior to the Split are affected by the Split. Note that the Surface used to create the Split is associative with the solid feature. Also note that the Split Direction can be reversed by clicking on the directional arrow in Geometry View. Explain that the Surface must fully cut across the solid features in the Part Body in order to create the Split. Otherwise, an error message is returned.

Surface Design

Thickening a Surface 1

2 Select the surface to be thickened. Surface to be thickened

Offset direction

!

3 Click OK to thicken the surface.

Instructor Notes:

Explain the process of creating a Thick Surface solid feature. Point out that this feature follows the same logic as discussed for the Split in its order of operation on the active Part Body. Note that the Offset Direction can be reversed by clicking on the directional arrow in Geometry View or the Reverse Direction button in the dialogue box. Also point out that two offsets can be specified for the Thick Surface (one in each direction).

Surface Design

Closing a Surface into a Body 1

2 Select the surface to be closed. Surface to be closed

3 Click OK to close the surface. Copyright DASSAULT SYSTEMES

\$

!

" #

Instructor Notes:

Explain the process of creating a Closed Surface solid feature. The same logic for order of operations in the currently active Part Body as described for Splitting and Thick Surface also applies here. Point out that the Surface being used to create the Solid Feature can have openings, but that they must be Planar Openings or an error will be returned.

Surface Design

Completing Geometry Recommendations

We will consider recommendations for creating a solid from surfaces.

Instructor Notes:

Surface Design

Creating a Solid Close Surface Surface geometry must have only planar openings for a solid to be successfully created with the Close Surface command.

The update error indicates an obvious non-planar opening or a slight gap between surface geometry.

Non-planar opening

Split the surface geometry with a plane to insure the opening is planar.

Slight gap between surfaces

Use the Preview in the Join command to check for gaps.

Instructor Notes:

Repair gaps with the Healing command. Repair gaps by modifying or re-creating the necessary surface geometry.

Surface Design

Completing the Solid in Part Design Recap Exercises 40 min

You will now do the following exercises Button Mouse

Instructor Notes:

Surface Design

Completing the Solid in Part Design Recap Exercise: Button 10 min

In this recap exercise you will: Create a Solid Button using Surface Geometry to define the shape Create two sketch profiles for designing solid parts Split the solid Apply Fillets Create Shell

Instructor Notes:

Surface Design

Completing the Solid in Part Design Recap Exercise: Mouse 30 min

In this recap exercise you will: Create a solid using Close Surface functionality Create Pads and Pockets Use the thickness command to provide thickness to surface and shell command to hollow a solid.

Instructor Notes:

Surface Design

Additional Reference Material Additional information can be found in the following reference material: Companion: Skillets: Editing Surface and Wireframe Definition Keywords: Edit, Element

Documentation: Books:

Mechanical Design Solution – Wireframe & Surface Design, Part Design Shape Design Solution – Generative Shape Design

Search String:

Split, Thick Surface, Close Surface, Solid

Instructor Notes:

Present the different Companion documents available for additional information and the on-line documents. NOTE: a demonstration is preferred to assist the students in locating the documents and showing at least one of them. It should be state that these sources of documentation do a go job in covering the features.

Surface Design

To Sum Up ...

You have seen CATIA V5 – Completing the Geometry in Part Design:

How to split a body with a surface How to thicken a surface How to close a surface into a body

Instructor Notes:

In the Summary, emphasize that the students have learned how to integrate surface development into Solid Bodies.

Surface Design

Modifying the Geometry You will learn how to modify the geometry after creation

What about Modifying the Geometry ? Editing Surface and Wireframe Definition Modifying Geometry Recommendations Modifying the Geometry : Recap Exercises Additional Reference Material To Sum Up

Instructor Notes:

Surface Design

What about Modifying the Geometry ? As the design matures, changes must be made to the geometry to reflect the current design. We will learn how to modify both wireframe and surface geometry.

Geometry can be modified by editing parameters in the definition or by modifying parent elements.

Key Points

When a parent element is modified, such as a profile curve, the surface created from the profile curve should be updated to reflect the change.

Modifying the parent element (point) …

Instructor Notes:

changes the profile curve and surface

Surface Design

Editing Surface and Wireframe Definition

You will learn how to edit the definition of wireframe or surface elements.

Element to edit

Instructor Notes:

Surface Design

Why Do You Need Editing? You can edit elements after part creation to change some of the parameters and thus make a new version of the part.

What about editing elements ? You can edit in the same way: wireframe elements surface elements

Editing the surface parameters.

Editing the definition of some points modifies the associated spline.

Instructor Notes:

Surface Design

Editing Elements 1

Activate the Definition box of the element: • Select the element then choose the xxx.object > Definition command. • Double-click on the element or on the element identifier in the specification tree.

2

Instructor Notes:

Modify the definition of the element by selecting new references or changing values.

3

Confirm element modification.

Surface Design

Modifying Geometry Recommendations

We will consider recommendations for modifying geometry

Instructor Notes:

Surface Design

Imposing a Value Range for Parameters To capture design intent, a value range can be imposed for a parameter. During modification, a message alerts the user if a parameter value is entered that is out of the specified range.

Imposing a value range

Right click in the parameter field

Key in Min and Max values

Value entered is out of range

Instructor Notes:

Surface Design

Identifying Parent and Child Elements For a more complex part, it may be difficult to determine which elements are driving the geometry that we want to modify. We can quickly determine the parents of an element and then edit those elements to modify the child. Terms: The element that depends on another element for its definition is called a child. The element that defines another element is a parent.

Determine parent or child elements

Double-click an object to view more parent/child elements

Point to the element on screen or in the tree

Instructor Notes:

Click the right mouse button and Parent/Children

Parents

Children

Surface Design

Modifying the Geometry Recap Exercises 20 min

Button and Mouse Exercises Topics covered:

Modify spline control points Modify a surface profile sketch Modify a surface fillet radius

Instructor Notes:

Mouse Exercises

Surface Design

Modifying the Geometry Recap Exercise: Button 10 min

In this step you will: Modify the Surface Shape of the Button Modify the Co-ordinates of the Spline Modify the radius of sketch used to design the side surface

Instructor Notes:

Surface Design

Modifying the Geometry Recap Exercise: Mouse 10 min

In this step you will: Modify the Wireframe geometry in order to change the surface shape and create more ergonomic solid Modify the Co-ordinates of the Top Spline control points Modify the fillet radius Modify several control points on the side spline

Instructor Notes:

Surface Design

Additional Reference Material Additional information can be found in the following reference material: Companion: Skillets: Updating A Part Keywords: Update, Local update, Edit

Documentation: Books:

Mechanical Design Solution – Wireframe & Surface Design Shape Design Solution – Generative Shape Design

Search String:

Edit, Modify, Definition, Wireframe, Surface

Instructor Notes:

Present the different Companion documents available for additional information and the on-line documents. NOTE: a demonstration is preferred to assist the students in locating the documents and showing at least one of them. It should be state that these sources of documentation do a go job in covering the features.

Surface Design

To Sum Up ...

You have seen CATIA V5 - Geometry Modification:

How to edit the definition of wireframe and surface elements.

Instructor Notes:

Surface Design

Using Tools You will become familiar with some tools used for managing wireframe and surfaces.

What about Using Tools ? Creating Datum Features Checking Connections Between Elements Updating a Part Using Tools: Recap Exercise Additional Reference Material To Sum Up

Instructor Notes:

Surface Design

What about Using Tools ? This section will show us tools that will help us become more efficient when creating shape geometry. Tools can help us copy elements instead of creating them again. Tools also allow us to directly create elements located on a certain plane or surface support.

Using tools will help us create shape geometry more efficiently.

Key Points

A tool is activated if it appears highlighted (usually orange colored) at the time a command is being used.

Tools are typically located on the horizontal toolbar in both the Generative Shape Design and Wireframe and Surface workbenches.

Tools are active

Instructor Notes:

Tools location

Surface Design

Creating Datum Features

You will learn how to create datum features

Instructor Notes:

Surface Design

Why Do You Need to Create Datum Features ? A datum feature is an element which has no link (history) with the elements used to build it (parent elements).

A datum feature is a non-modifiable element. Even if you change the definition of its parent element(s) the datum feature remains unchanged.

If you click on the Create Datum icon only the element to be created will be defined as datum feature.

If you double-click on the Create Datum icon all the elements will be defined as datum features until you click the icon again to de-activate it.

Instructor Notes:

Explain the nature of a Datum feature. Discuss why you might want to create a Datum feature instead of a feature with a normal Parent / Child relationship.

Surface Design

Checking Connections Between Elements

You will learn how to check connections between surfaces or between curves.

Instructor Notes:

Surface Design

Checking Connections Between Surfaces 1

Select the Connect Checker Icon

2

Multi-select the two surfaces between which you want to check the connection

3

Choose the Analysis Type : Distance, Tangency or Curvature

Note the Maximum values between the two surfaces.

Instructor Notes:

Explain the components of the Quick Violation Analysis dialogue box. Note how changing the values in the combo boxes next to the color code for Distance, Tangency and Curvature will accordingly adjust the graphic display of these color on the Surfaces being examined. Explain how Maximum Gap affects the checking of Surfaces that are not connected to each other. Point out that the results of the Surface Connection Analysis is saved in the Part tree and can be reopened later on.

Surface Design

Checking Connections Between Curves This tool allows you to detect the point, tangency, curvature and curvature tangent discontinuities on curves.

Distance Analysis

Tangency Analysis Curvature Analysis G0 analysis G2 analysis

The G0 discontinuities are displayed on the analyzed curve.

G1 analysis

The G1 discontinuities are displayed on the analyzed curve.

Curvature Tangency Analysis

The G2 discontinuities are displayed on the analyzed curve. G3 analysis

The G3 discontinuities are displayed on the analyzed curve.

Instructor Notes:

Explain the options available in the dialogue box for Curve Connection Checker. As with the Surface Connection Checker, options are available to change the color visualization based on values set in the dialogue box. Note that a Curve Connection Analysis feature is stored in the Part Tree when this tool is used.

Surface Design

Updating a Part You will learn how to update your part in case you have chosen the manual update mode.

Part to be updated

Instructor Notes:

Surface Design

Why Do You Need to Update a Part ? You can choose to work in the Automatic or Manual update mode. If you work in the Automatic mode your part is automatically updated. If you work in the Manual mode you can update your part whenever you want.

In the Manual mode you know that the part needs to be updated when:

The Update symbol appears next to the part name.

The Update icon is available.

The part is displayed in bright red.

Instructor Notes:

Explain the difference between Automatic and Manual update Mode. Discuss why you might want to work in one mode or the other. Note the Part Tree and Geometry displays when a part is changed and Manual Update mode is in effect.

Surface Design

Updating a Part: Settings The Automatic Update mode is the default mode set in the Options. You can change the default update mode in Tools + Options + Infrastructure+Part Infrastructure.

Note that the chosen update mode is the same in Wireframe and Surface Design and in Part Design.

Let ’s see now the way to update a part...

Instructor Notes:

Explain the Options available for controlling Update behavior in a Part Document. Note and discuss the other Options that can be activated under Update. Stop Update on First Error Synchronizing External References during an update Activate Local Visualization

Surface Design

Updating a Part 1

Set the update mode to Manual.

2 Perform a modification for which an update is required.

Here the spline and the surface need to be updated. Initial part

3

Modification of a point

Update the part to display the new spline and surface: • click on the Update icon in the Tools toolbar

• select Edit + Update in the menu bar Resulting part

• select the Local Update option from the contextual menu positioning the cursor on the Part identifier If you position the cursor on a feature and select Local update from the contextual menu only the feature is updated.

Instructor Notes:

Explain the process of Part change and Manual Update as shown here. Have the students experiment with different Options for controlling the Update if you have time.

Surface Design

Using Tools Recap Exercise: Surface Check Exercise 10 min

In this exercise you will: Analyze a set of surfaces for deviation gaps, non tangency, and curvature value. Perform a quick analysis for summary of results Perform a detailed analysis and also change the color scale Display the results with ‘Comb’ and ‘Information’ displays.

Instructor Notes:

Surface Design

Additional Reference Material Additional information can be found in the following reference material: Companion: Skillets: Shape Design Common Tools Keywords: Stack, Command

Documentation: Books:

Mechanical Design Solution – Wireframe & Surface Design Shape Design Solution – Generative Shape Design

Search String:

Cut, Copy, Paste, Delete, Datum, Working Support, Update, Connection

Instructor Notes:

Present the different Companion documents available for additional information and the on-line documents. NOTE: a demonstration is preferred to assist the students in locating the documents and showing at least one of them. It should be state that these sources of documentation do a go job in covering the features.

Surface Design

To Sum Up ...

You have seen CATIA V5 - Using Tools:

How to cut, copy, paste or delete elements, How to create datum features, How to work on a support and snap to a point, How to update a part manually, How to check connections between curves or surfaces

Instructor Notes:

Surface Design

Master Exercise: Mobile Phone In this exercise you will create 'Mobile Phone' model using the tools of Wireframe and Surface Design workbench.

Mobile Phone: Presentation Mobile Phone (1): Creating Wireframe Geometry Mobile Phone (2): Creating Basic Surfaces Mobile Phone (3): Trimming and Joining the Body Surfaces Mobile Phone (4): Creating the Part Body Mobile Phone (5): Modifying the Geometry

Instructor Notes:

Surface Design

Mobile Phone Master Exercise Presentation 65 min

In this exercise you will build Mobile Phone body using Wireframe, Generative Shape Design, and Part Design Workbenches. Here you will first create all the necessary wireframe elements. After that you will create surfaces from these wireframe elements Then you will perform operations on these Surfaces to get a single homogenous surface. Using this surface you will create a part from it. You will finally optimize your design by modifying some of its specifications.

Instructor Notes:

Surface Design

Mobile Phone Step 1: Create the Wireframe Geometry 15 min

In this step you will create the basic wireframe elements.

Create Points Create Splines Create Projections Create 3D Circles

Instructor Notes:

Points

Circle

Surface Design

Mobile Phone Step 2: Create the Basic Surfaces 20 min

In this step you will create the basic Surfaces from the wireframe elements created previously to build the part.

Create Sweep Surfaces Create Blend Surfaces Create Extrude Surfaces

Instructor Notes:

Surface Design

Mobile Phone Step 3: Trimming and Joining the Body Surfaces 15min

In this step, you will perform operations on the surfaces that you have created to get a single uniform surface.

Create Joins Trim Surfaces Cerate symmetrical surfaces

Instructor Notes:

Surface Design

Mobile Phone Step 4: Creating the Part Body 10 min

In this step, you will create the Part from the surfaces you have created, by accessing the Part Design Workbench

Create a Closed part from a surface Apply Fillets

Instructor Notes:

Surface Design

Mobile Phone Step 5: Modify the Geometry 5 min

In this step you will Modify the overall Shape of the Part by changing the parameters of the 3D reference elements.

Edit the values of the 3D reference elements Study the impact of these modifications

Instructor Notes:

Surface Design

In this course you have learned how to design and modify parts using wireframe geometry and basic surfaces.