Sep 19, 2008 - CATIA Product Design Expert ... First load all the components from Companion into CATIA V5 and save them ... following assembly constraints:.
Publication Recap Exercise 1. Webcam Detailed Steps Objective: In this exercise you will experiment the benefits of Publication while replacing a component, in terms of positioning constraints and in design in context. Time: The design document has allocated 25 minutes to complete the project. To assist you if you need, a series of detailed step-by-step directions has been provided on the following pages. The detailed instructions below give you our recommendations to complete the scenario: 1.1 -
Assemble the webcam:
Advise for Companion users: First load all the components from Companion into CATIA V5 and save them into a temporary directory of your choice. Then insert the specified components from this directory. •
Create a new Product and rename it "Webcam".
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Insert in it "Existing component": "Inferior_Body.CATPart" and fix it with the "Fix" constraint.
•
"Insert Existing Component": "Camera_Assembly.CATProduct" in "Webcam". Create the following assembly constraints:
Coincidence between xy plane of "Inferior_Body" and xy plane of "Lens_Support". Coincidence between zx plane of "Inferior_Body" and zx plane of "Lens_Support". Contact between interior face of "Inferior_Body" and published "Lens_Support". •
of
"Insert Existing Component": "Support.CATPart" in "Webcam". Create the following assembly constraints:
Coincidence between zx plane of "Inferior_Body" and zx plane of "Support" Coincidence between
of "Inferior_Body" and of "Support".
•
"Insert Existing Component": "Base.CATPart" in "Webcam". Create the following assembly constraints:
Coincidence between
of "Support" and
of "Base".
Offset of (-28mm) between xy plane of "Support" and xy plane of "Base".
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1.2 -
Design the cover in context:
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Go in "Tools> Options" panel and check that "Keep link with selected object" option is activated:
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Create a new part and name it "Top_Body".
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Create coincidence constraints between xy, yz and zx planes of "Inferior_Body" and "Top_Body". Activate "Top_Body" component in order to design the cover.
• •
Click on "Shaft" icon and select as profile "External_Profile" sketch in "Inferior_Body" structure. Make sure an external reference is created.
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Then fill in the fields of the Shaft Definition panel as shown on picture below:
•
Click on Shell icon
. Select the planar face as "Face to remove".
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•
Create the Sketch below with zx plane as sketch support. Notice that the upper line of the rectangle is coincident to 3D plane "Splitting_Plane" that you will find in "Inferior_Body". Make sure that an external reference is created while selecting this plane.
•
Click on Slot icon . Select previous sketch as Profile and as Center Curve select "Webcam_Section" in "Inferior_Body". Make sure that an external reference is created for "Webcam_Section".
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Select yz plane in the specification tree and click on Hole icon in order to create a hole centered on part origin. Create a simple hole of Diameter 15mm and Depth 10mm. Reverse direction if necessary.
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1.3 -
Try to replace the inferior body:
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Use Save Management command to save the entire product.
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Right-click on "Inferior_Body" and select "Replace Component…" command in the contextual menu". In the "File Selection" panel select "Spherical_Body.CATPart". Validate the "Impacts On Replace" panel.
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In case you are working with Companion, first load "Spherical_Body.CATPart" from Companion into CATIA V5, and then select "Replace Component In Session" option in "Inferior_Body" contextual menu. Notice that the Part Number of the component in the specifications tree has changed but not its instance number. Notice that some assembly constraints are broken and that the external constraints of "Top_Body" are disconnected. Close the Product without saving the modifications.
• • •
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1.4 -
Publish "Inferior_Body" reference elements and recreate the links:
• • • •
Reopen "Webcam.CATProduct". Delete "Top_Body" component from the specifications tree. Activate "Inferior_Body". Open "Tools> Publication…" menu.
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In "Inferior_Body", select the elements that were used in step 2 to design "Top_Body": "External_Profile", "Splitting_Plane" and "Webcam_Section".
• •
They are added to the list of published elements. Select also the elements that were used in step 1 in assembly constraints: "Support_Axis" and the internal face of the solid (highlighted face on picture below).
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•
Modify the Publication name of the internal face by selecting it in the Publication panel and then clicking again on its default name. Rename it "Internal_Face".
• •
Activate root product. Delete the constraints that were broken in step 3:
Surface contact between "Inferior_Body" and "Camera_Assembly" Coincidence between axes of "Inferior_Body" and "Support" •
Recreate these constraints using this time the published elements of "Inferior_Body":
Contact between published
of "Inferior_Body" and published
of "Lens_Support". Coincidence between published
of "Inferior_Body" and
of "Support". •
Insert a New Part in "Webcam" named "Top_Body_Publication".
Activate "Top_Body_Publication" in order to design the cover again, but this time using the Published elements of "Inferior_Body.1":
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between xy, yz and zx planes of "Inferior_Body" and
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Click on "Shaft" icon and select "External_Profile" in "Inferior_Body.1" Publications node. Make sure an external reference is created.
Then fill in the fields of the Shaft Definition panel as shown on picture below:
•
Click on Shell icon
. Select the planar face as "Face to remove".
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•
Create the Sketch below with zx plane as sketch support. Notice that the upper line of the rectangle is coincident to 3D plane "Splitting_Plane" that you will select in "Inferior_Body" Publications node. Make sure that an external reference is created while selecting this plane.
•
Click on Slot icon . Select previous sketch as Profile and as Center Curve select "Webcam_Section" in "Inferior_Body" Publications node. Make sure that an external reference is created for "Webcam_Section".
•
in order to create a hole Select yz plane in the specification tree and click on Hole icon centered on part origin. Create a simple hole of Diameter 15mm and Depth 10mm. Reverse direction if necessary.
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Save the whole Product using "Save Management" command.
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1.5 -
Replace the Inferior Body
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Open "Spherical_Body" and check that it contains the same publications with exactly the same names than "Inferior_Body" (also check uppercase). Note that the ordering of the Publications as no importance. Rename the Publications of "Inferior_Body" and save the Product again if necessary.
•
Right-click on "Inferior_Body" and select "Replace Component In Session" command in the contextual menu". Validate the "Impacts On Replace" panel. Update the Product.
• • •
This time, the geometry of the cover has adapted to the spherical shape of the new inferior body: the external references of the cover have automatically been reconnected to the published elements of the replacing part. The assembly constraints have also been automatically reconnected to "Spherical_Body" thanks to Publication.
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