1. Doing an Assembly – Catia’s Answer IE 1225 Introduction to Design & Manufacturing Dr. Richard Lindeke, Ph.D.

2. Issues we will explore: Using the Product Tree Part Command allows parts can be inserted into the tree and designed “on the fly” Components which are coupled into the “CATProduct” but don’t exist as a separate entity in its own file Existing Component is used to insert an existing part or assembly into the current Product Sub-Assemblies are previously developed Assembled Products that can be inserted into a current product “all at once”

3. Considering Assembly Constraints: Coincidence Constraints: aligns axes, planes and points Contact Constraints: a tool for creating contacts between 2 planes or surfaces Offset Constraint: defines a desired offset distance between two elements Angle Constraints: A way to define an angular relationship between two elements

4. Considering Assembly Constraints: Fix Component: A way to FIX a part “in space” so that it will always remain there. Other parts can be constrained relative to a Fixed component Fix Together: Fixes two parts together (forever) Flexible/Rigid Subassembly: in a flexible sub, parts and components can be moved regardless of the fact if it (or they) are the active component

5. More Considerations: Use Save Management commands because of the several links within the root tree Save or save-as individuals in the Save Management window We can also just “Save All” for a full update When modeling because of constraining issues, parts must have tolerenced dimensions added

6. We Finish with an Assembly:

7. From Which we Make an Exploded Product Drawing Note: The Product is highlighted – We can explode and assemble!

8. Building An Assembly Start Work in the Assembly Workbench We begin with a “Root” CATProduct We can create “Components” of the assembly that exist only within the “Root Files” We can inport Existing Components to the Assembly (parts or sub-assemblies created earlier) W/ or W/O positioning We can create Parts for the Assembly “on the Fly” We can create “Instances” or duplicates of parts We can create Numbers or Letters to Identify parts of an Assembly – for BOM needs We can “Manage Representation” (names, associations, etc.) of the components of an assembly We can Bring in Catalog – or standard – components to our assemblies like bolts/nuts/pins, etc.

9. Because Assemblies are Multi-component products get in the habit of ‘SaveManaging’ them and consider using Folders to save all of the components and parts required

10. Lets Get Started:

11. Using Ass’bly I & properties to name it then Add Part ICON to create Part1.1 under it & then Properties/ set Instance Name to ToolPostBody

12. Draw a Profile on ZX plane as seen

13. Pad the Sketch to Dimension on Pg 5.1-7 Add Fillets to Sides – as specified in Drawing Pg. 5.1-7 too!

14. Draw & Contrain the Profile on Large side – to pocket

15. Add Main Thru Hole – Toleranced:.502 -.504; Positioned as seen

16. Clicking Tolerance ICON (on hole) lets us set the dimensions

17. Add 2 Threaded Holes – Finally Counterbored Hole Positioned as seen:

18. Make Face Threaded Holes and Add Material (Cast Iron)

19. This Part Is Finished – Save Manage!!

20. Add a Second Part (to ToolPost Assembly)

21. Draw a Profile for the Wedge – as Specified – note Angle is 160!

22. Before Setting Slot Width – enter Tools … Options: Set Tolerance Default to +0 -.012 Then set Slot Width 0.19; Then turn Default Tolerance Off! After Resetting Def. Toler.; Exit Sketcher and Pocket “Up to Last” Then Save Manage

23. After Saving: Show Part 1 Attach the Compass to The Wedge and Move it Away from the Tool Post Body Part Note: The Compass is Attached to the Wedge – only it is moving! When we finish Click on the Red Box and drag it “Home (upper Right Corner of View)

24. Make a 3 rd Part – BOLT- Make it as a Shaft; Careful of Tolerance – Then Sketch and Pad the Head

25. Then Thread the End: ½ x 13 UNC for 1.25”

26. After Chamfer its End and Save Managing for the Bolt; Un-Hide The Body & Wedge and Reposition the Bolt

27. Standard Parts can be added We highlight the Assembly Then Click Tool and Mech Std Parts – ASME, ANSI Inch Catalogs

28. The set screws are inch Size Screws – use ¼ x 20 1.73” headless – modify for proper length and End Form (Edit Formulas)

29. After Adding it We can change its Name – Set Screw 1 (or not) then save manage

30. A Second Headless Set Screw can be added By Copying this: Rt. Click it.. Copy Then Rt. Click Tool Post Product and … Paste – Move it where we desire

31. Add The ASME Nut (washer type) and Washer – position them Then Draw in the Rest of the Components: The Tool Post Screw (and make a copy); Then Adj. Screw; Finally Slotted Washer and Adjustor Nut

32. Once all components are Drawn and Saved We add Assembly Constraints – The Heart of the Task! First A Contact Constraint Between The Bottom of the Wedge and The top of the Sloped Surface in the T.Post Body

33. After Contact Constraint Between Wedge and T.P. Face A very Useful Offset Constraint Between the Front Face of the Body and The Wedge

34. Anchor (FIX) the Tool Post Body Then “Up Date” to Bring the Wedge into Position

35. Apply Coincidence Constraints to the Axes of the Set Screws and Body Holes – And Offset Constraint To Back of Body and “Screw Slots”

36. Add The Rest of The Components & Their Constraints for Assembly on Your Own

37. I had previously made and saved the ToolPost Screws – So I added them as components w/ Positioning They need to have coincidence and Offset Constraints applied for proper “Posing”

38. After the Copied Screw was constrained: