CATIA Mold Tooling Design

Jan 19, 2009 - Select new Product in the specification tree (orange highlight) ... Page 5 ... Select in the dialog box the design table icon corresponding to ...
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CATIA Training

CATIA Mold Tooling Design Detailed Steps

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Version 5 Release 19 January 2009 EDU-CAT-EN-MTD-FS-V5R19

CATIA Mold Tooling Design

Detailed Steps

Table of Contents Master Exercise: Phone Handset ........................................................................................................... 3 1. Creating a new Mold........................................................................................................................ 3 2. Creating Components.................................................................................................................... 11 Creating Injection Features ............................................................................................................... 27

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CATIA Mold Tooling Design

Detailed Steps

Master Exercise: Phone Handset 1. Creating a new Mold In this step, you will: • Access workbench Mold Tooling Design • Create a new Product • Insert existing Molded Part • Select a Mold Base in a Catalog • Position the Molded Part in the Mold Base • Split the Core Plate and the Cavity Plate 1.1 - Enter workbench Mold Tooling Design to start a new Product :

1.2 - Insert existing Molded Part : • Select new Product in the specification tree (orange highlight) • Activate function Insert / Existing Component…

• Select file : MoldedPart.CATPart :

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CATIA Mold Tooling Design

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• In Geometrical Set PartingBody, show PartingSurface :

1.3 - Select a Mold Base in a catalog : • Click icon Create a new mold:

• Click Catalog icon in dialog box Create a new mold… • Double-click successively reference Dme, then N3050-1 in the Catalog browser dialog box (variant without overhang on Clamping Plate and Setting Plate). A bounding rectangle corresponding to the size of the Mold Base is displayed.

• Click OK to validate : a graphic preview of the complete Mold Base is displayed and the dialog box Create a new mold…is updated with the list of plates and default dimensions corresponding to this reference :

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CATIA Mold Tooling Design

Detailed Steps

• Select Left View to better check the positioning of the part and the thickness of the Core and Cavity Plates : the plates are too thin and the position of the Part should be adjusted to fit in the overlap area between Core and Cavity Plates.

• Select in the dialog box the design table icon corresponding to Cavity Plate, select reference whose height = 86mm, and click OK to validate

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CATIA Mold Tooling Design

Detailed Steps

• Proceed similarly to adjust Core Plate height to 86 mm and Riser Bar height to 106 mm :

• Click OK to validate : you can see that sub-product Mold has been created in the specification tree. You can also notice that the Mold Base comes with many DME-predefined location points to help position other components : circle points for guiding or locating elements (Leader Pins, Sleeves, Bushings), cross points for fixing elements (Cap Screws), star points for specific components (Locating Ring).

1.4 - Adjust the position of the Molded Part in the Mold Base : • In the Molded Part, unfold tree branch Axis Systems : you can see that there is a Local Axis system in the Part, but it is not current, therefore it has not been used by the application to

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CATIA Mold Tooling Design

Detailed Steps

define the positioning of the Molded Part in the Mold Base. Instead, the main planes of the Molded Part were used.

• Put in Show mode the main planes of the Molded Part : you can see that their origin is positioned at equal distance between the top of the Cavity Plate and the bottom of the Core Plate (which are overlapping) : this is the default positioning which has automatically been performed by the application. Put the plane back in NoShow.

• The position of the Molded Part has to be adjusted to place it in the overlapping area of the Core and Cavity Plates. Click icon Manipulation :

• Click icon Top View. You can see that the Parting Surface completely splits the Core Plate, therefore no further positioning is required along X and Y axes.

• Click icon Left View. Select Z-axis icon in panel Manipulation Parameters and drag Molded Part along Z axis to position it in the overlapping area of the Core Plate and Cavity Plate. Validate.

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CATIA Mold Tooling Design

Detailed Steps

1.5 - We will now split the Cavity Plate to shape it to the form of the Molded Part. We will use a splitting surface already prepared. • In the specification tree of the Molded Part, unfold Geometrical Set PartingBody. Put PartingSurface in NoShow and put CavitySurface in Show.

• Activate (MB3) contextual menu of the Cavity Plate and select function Split component… :

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CATIA Mold Tooling Design

Detailed Steps

• The system proposes CavitySurface as default value for the splitting surface : if necessary, activate option Display direction to check the orientation and reverse it if needed to keep the upper side of the plate. Click OK in the Split dialog box.

• Note that a new Product and a new Part (named Product1_InjectionSide and TlgItf_InjectionSide and) have automatically been created to manage contexts in subassembly Injection Side : the split operation has made CavityPlate contextual to MoldedPart.

1.6 - Proceed similarly for the Core Plate, using surface named CoreSurface

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CATIA Mold Tooling Design

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1.7 - The final result should look as shown. Hide the Molded Part, then alternatively hide InjectionSide and EjectionSide to check the result visually.

1.8 - Close the document without saving it if you want to use existing prepared data for the next step, or keep it opened if you want to continue with it.

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CATIA Mold Tooling Design

Detailed Steps

2. Creating Components In this step, you will: • Create Guiding components : Leader Pins • Create Fixing components : Cap Screws • Edit the definition of existing Cap Screws • Create Ejection components : Ejector Pins • Split Ejector Pins You will learn how to select, position and edit Components. 2.1 - If you have not kept the result of the previous step, open existing Product : Creating_Injection_Features_Step2_Start.CATProduct

2.2 - Create Leader Pins : • Click icon Add Leader Pin. Click catalog icon in panel Define Leader Pin in order to display the catalog panel.

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CATIA Mold Tooling Design

Detailed Steps

• In dialog box Catalog Browser : Leader Pin, double-click reference Dme to get the list of references.

• Double-click reference LeaderPin_FSC • You can see that the system has applied a predefined filter to display only the references of this type which are relevant. In this case, the filter applied (D=20mm) corresponds to the diameter recommended by the supplier for this variant of Mold Base.

• Click reference FSC-20-36-146 :

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CATIA Mold Tooling Design

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• Pick one of the predefined points located in the corner of the ClampingPlate in order to position the first instance of the Leader Pin :

• You can see that the system has automatically recognized all four predefined points intended for positioning the Leader Pins. All instances are highlighted in red, which means that all of them are active : any further positioning operation will therefore apply to all of them simultaneously.

• Click button Reverse Direction to re-orientate the Leader Pins.

• Uncheck button Manage All in the dialog box. Only one instance stays active (red highlight), the other ones become inactive (they turn to green) : any positioning operation will then apply only to the current active instance.

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CATIA Mold Tooling Design

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• Move the mouse over the vertical green arrow of another instance : this new instance becomes the active one (red highlight).

• Activate again button Manage All to make all instances active. Note that you can do any number of switch operations and positioning operations in order to reach the desired result for all instances. Note that option Several Instances per reference is active : the four Leader pins will therefore be created as instances of the same single reference.

• To define the Leader Pin drillings to be applied to the Mold Base, select ClampingPlate as plate Drill From, and CavityPlate as plate To. You can select them graphically or in the specification tree. • Note that Father Product, set by default to the current active Product (top Product called Product1), has automatically been switched to InjectionSide when you have picked Drill From = Clamping Plate : InjectionSide is the father sub-assembly of ClampingPlate.

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CATIA Mold Tooling Design

Detailed Steps

• Click OK in the dialog box to validate the creation. You can see that all four instances of the Leader Pin have been created, together with their associated holes in the plates (hide Leader Pins to see the drillings). They have been created in the specification tree in sub-assembly InjectionSide, which is the location of the Drill From plate (ClampingPlate).

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CATIA Mold Tooling Design

Detailed Steps

• Note also the automatic creation of Technological Results in the ClampingPlate, conveying the technological information of the DrillHoles of the LeaderPins impacting the plate.

2.3 - Insert Fixing Component : Cap Screw

• Click icon Add Cap Screw

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CATIA Mold Tooling Design

Detailed Steps

• Select one of the predefined 3D points for Cap Screws located in the SettingPlate. In panel Define CapScrew, select field To, then pick CoreSupportPlate in the 3D viewer. In tab Specifics activate Diameter and enter value 12mm. Keep default value for minimum thread engagement ratio (1.5 * Diameter)..

• Click icon Catalog in the dialog box . Double-click provider Dme, then type CapScrew_M. You can see that the system has automatically pre-selected a subset of Screw variants by using a filter on their length and their diameter. This filter has been computed by using the elements previously defined : positioning point, target drilled plate (CoreSupportPlate), diameter, minimum thread engagement ratio.

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CATIA Mold Tooling Design

Detailed Steps

• Select reference M12*140. Define Drill From = SettingPlate. Set W = -10mm. Click button Between From and To in order to remove both Ejector Plates from the list of drilled elements computed by the system : this will avoid to create unnecessary Boolean features in these plates (they are not geometrically impacted by the screws) and will also avoid to create an unnecessary Part Interface in Ejector System to manage the context dependencies. Validate creation.

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CATIA Mold Tooling Design

Detailed Steps

• Hide one of the screws. You can see that SettingPlate and Risers have been drilled with standard holes, while the last plate (CoreSupportPlate) has been bored with a threaded hole.

2.4 - Change the size of the Cap Screws : • Switch to Left View. Select a CapScrew instance in the specification tree (EjectionSide), activate its contextual menu and select function Edit CapScrew component :

• Select tab Parameters in dialog box Edit CapScrew, activate design table icon corresponding to parameter L (length) and select reference M12*150. You can see that all impacted plates have turned red (update needed). COPYRIGHT DASSAULT SYSTEMES

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CATIA Mold Tooling Design

Detailed Steps

• Validate modification : you can see that all four instances of the Cap Screw have been updated simultaneously.

2.5 - Create Ejector Pins • To facilitate the visualization and the positioning of the Ejector Pins, hide InjectionSide.

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CATIA Mold Tooling Design

Detailed Steps

• Double-click part EjectorPlateA in the tree. Make sure that Geometrical Set.2 is the current active body (Define In Work Object).

• Using the keyboard up/down arrows to “get through” the lower Plates, select the bottom face of EjectorPlateA and click icon Sketcher

• In Tool Bar Sketch Tools, make sure option Snap To Point is de-activated. If necessary, click icon Normal View to have a view from the top of the Mold instead of the bottom.

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CATIA Mold Tooling Design

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• Double-click icon Point, define several points approximately as shown, then exit Sketcher. These points are going to be used to locate Ejector Pins.

• Double-click top Product to go back to workbench Mold Tooling Design. • Click icon Add Ejector Pin and select in Hasco catalog the reference EjectorPin_Z441. Note that the system has applied as filter the distance between the bottom of EjectorPlateA and the top of the rough CorePlate (i.e. without taking into account the split of this plate).

• Double-click proposed reference Z441/2x250 and pick one of the points of the sketch previously created. You can see that the system has created and positioned an Ejector Pin on each point of the Sketch.

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CATIA Mold Tooling Design

Detailed Steps

• Note that option Several Instances per Reference is not active (the value shown is the one defined in the Settings).This will ensure that each EjectorPin is created as a reference and can therefore be handled individually for splitting purposes later on.

• Drill from has automatically been set to EjectorPlateA (which contains the Sketch selected for positioning). Define drill To = CorePlate.

• Zoom onto the top of the Ejectors. You can see that a white dashed line in the preview shows the height of the clearance hole associated to each Ejector Pin. The length of this hole is not appropriate : the Ejector Pins would not fit in closely with the Core Surface. But the length of the fitting hole will later be automatically adjusted by the Split operation to the value defined in parameter Offset_Parting (here 10 mm).

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CATIA Mold Tooling Design

Detailed Steps

• Validate creation of the Ejector Pins. All the references have been created in sub-assembly EjectorSystem

2.6 - Split the Ejector Pins : • Multi-select the Ejector Pins in the specification tree and activate function Split Component in the contextual menu.

• Keep default value proposed by the system (CoreSurface) as splitting element. If necessary, reverse the splitting orientation by clicking one of the arrows in the 3D viewer in order to have them point downward to keep the appropriate side of the Ejector Pins after split.

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CATIA Mold Tooling Design

Detailed Steps

• Validate and zoom onto Ejector Pins area to check the result. Note that Split operation has automatically adjusted the fitting length of each EjectorPin to take into account the value defined in parameter Offset_Parting (use Measure Between for checking if desired).

• Show External Reference element in the EjectorPin and note that operation Split Component has automatically restricted the splitting surface of the Ejector to a small area around it (it has not used the full surface). The restricted surface in each Ejector comes from a second Part Interface automatically generated by the system and containing the reference Split surfaces generated by the system in the new Part TlgItfSplit generated at root level

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CATIA Mold Tooling Design

Detailed Steps

2.7 - Close the document without saving it if you want to use existing prepared data for the next step, or keep it opened if you want to continue with it.

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CATIA Mold Tooling Design

Detailed Steps

Creating Injection Features In this step, you will: • Create a Gate • Create a Runner • Create a Coolant Channel 2.8 - If you have not kept the result of the previous step, open existing Product : Creating_Injection_Features_Step3_Start.CATProduct.

2.9 - Hide EjectorPins. In MoldedPart, show only curve named PartingLine.

2.10 - Create a Gate : a. Click icon Add Gate

b. Create the location point of the Gate : define the point as a Point On Curve, select PartingLine (in red) as support curve and pick a point approximately as shown below. Click Preview in dialog box Point Definition to check the position. Validate creation.

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CATIA Mold Tooling Design

c.

Detailed Steps

You can see that the point has been created in the Molded Part in a Geometrical Set named GateBody and that it is graphically marked as a yellow square. You will now enter the geometric definition of the Gate in panel Gate definition.

d. Keep default Stamp side proposed by the system (Core). Define Gate parameters : in dialog box Gate definition, click catalog icon and double-click successively type SideGate, then SideRound, then Round, and set value Radius = 1 mm. You can see that a preview of the Gate is displayed (in red). Validate the creation.

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CATIA Mold Tooling Design

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2.11 - Create a Runner : e. Double-click in the specification tree Part MoldedPart to make it the current Part. f.

Create a new Geometrical Set. Select plane XY and enter Sketcher. Make sure grid option icon Snap to Point is de-activated.

g. Click icon Profile, and draw a profile approximately as shown, ensuring tangency continuity all along (use for example dialog box Constraint Definition for this purpose). This is mandatory to ensure a correct projection of the sketch onto PartingSurface when creating the Runner in the next step.

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CATIA Mold Tooling Design

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h. Ensure coincidence between the Gate point (yellow square) and the extremity of the Runner : multi-select them, activate dialog box Constraint Definition and activate Coincidence.

i.

Now exit Sketcher, and double-click top Product in the Specification tree to come back to workbench Mold Tooling Design.

j.

Click icon Add Runner. Set Stamp = Core only, switch section type to Oval, set Radius value = 2.5 mm and select the new sketch as Layout. Validate the creation. Hide MoldedPart to check the result more clearly.

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CATIA Mold Tooling Design

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2.12 - Create a Coolant Channel in the Core Plate : k.

In sub-assembly EjectionSide, double-click Part CoreCooling to make it active. Create a new Geometrical Set..

l.

We are now going to create a sketch of lines for the Cooling pipes. Click icon Plane, select type Offset from plane and select CoreCooling plane XY as reference plane. Adjust the position e.g. by dragging the green arrow. Validate creation.

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CATIA Mold Tooling Design

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m. Select the new plane, click icon Sketcher, create successively two lines as shown, ensuring coincidence between the extremities and the lateral faces of CorePlate :

n. Exit Sketcher and switch back to workbench MoldTooling Design. o. Select the new sketch in the tree, then click icon Add Coolant Channel. Two pipes are displayed according to the location of the sketch lines.

p. Keep default values. Validate creation of the Coolant Channel. Hide the support Sketch to better check the result. You can notice that counterbored holes are present on one side (corresponding to first point of sketch lines) to prepare further insertion of Plugs.

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CATIA Mold Tooling Design

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q. We are going to edit the definition of the Coolant Channel. Show again the support sketch, double-click it and modify it as desired. For example, drag one of the lines in a different position.

r.

Exit Sketcher and double-click the top Product to update the assembly : the Coolant Channel has followed the line in the new position.

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CATIA Mold Tooling Design

Detailed Steps

s.

Close without Save.

t.

The final result is available in \MasterExercise\Step3\End\Product1.CATProduct.

The end.

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