Wednesday, June 23, 2010

Best Practices for CATIA V5

There is a great thread for CATIA V5 Users:

I've compiled the complete list of suggests here:

1 Never make a plane from a solid face! Reason being is that if the solid changes, it can affect the plane which can snowball into a huge mess of errors.

2. (for managers) Never purchase Catia, and expect to implement it, and get full functionality, without TRAINING, and I mean professional training.

3. Never make geometry without knowing what the 'In Work' object is.

4. Never open a R18 file in R19, and accidently save it.

5. Never use File + save + Propagate directory, as a substitute for file and directory structure management.

6. Never alter the Customer model

7. Don't do fixed bid work for less than the going contract hourly rate. To do so is just plain self torture.

8. Never do fixed bid NC programming

9. If you ignore #8 .....Never do fixed bid NC programming, for an new customer, without a signed off preplan.

10. Never Mix hybrid and .........

11. Never trust that hotfix/SP will fix the problem you reported on first round without any additional problems...

12. Leave fillets out of sketches and make them as dress-up features operations except, curves that define major features of the design should be included in the sketch.

13. Never release a service pack, to the population, before a major test regiment

14. Never load a service pack, before a major deadline.

15. Never skip going to a COE annual Conference

16. Never do nothing but whine and complain about CATIA. Sure it's fun to poke at it, and have a good laugh at DS's expense. The reality is, as Roger says: ::CATIA keeps getting better all the time"

17. Never duplicate geometry within a sketch. Keep sketches simple, and only define a single profile. Use Pattern to duplicate the profile's feature

18. Never link to anything that isn't published
19. Never use Faces, Edges, or Vertices to create new geometry. You can use the, but always create an EXTRACT element first.

20. Never exit a sketch unless everything is fully constrained. (never exit if geometry is white - everything should be green or yellow)

21. Never exit a sketch without first doing a sketch analysis.

22. Avoid using Red. Catia uses Red to 'warn'. It can become confusing.

23. Don't use translate/rotate/scale in normal design. They are useful if you get data from other CAD, but other changes should happen with changes of part specification, not by adding these commands.

24. Don't try to do everything in one part like V4. Learn Products and do your work in your own CATPart.

25. Don't use the V4 method part modeling; don't make a body and pad of every solid feature and boolean Add or Remove the body to the part. V5 features are automatically added or removed, making boolean operations unnecessary for basic part design. Use boolean operations only for grouping and special situations.

26. Don't turn on the Datum mode when making surfaces, to create isolated surfaces like in V4. Keep the parent/child relationships to make it easy to modify surface models.

27. Don't blindly create all sketches as positioned just because you heard it was better. If you do create positioned sketches, make sure you position them properly. Positioned sketches are extremely useful but aren't required in a lot of situations. (Floating sketches have their own set of issues.)

28. Use "Positioned Sketch"

29. In general: The rule of one Physical Part = one CATIA Part. Body is not Part, it's Body. (Exceptions: e.g.: Over-molded parts.)

30. If you create Contextually linked part (part with contextual links) Position the part to common origin. Typical way of getting an assembly level update cycle is:
• Part is positioned with constraints that create a Positional link between geometry of this part & other parts
• Part has contextual links that affect to this very same geometry
èeasily there is a conflict of geometry position versus geometry shape... èUpdate cycle or impossible to update.
èIf you create contextually linked part, just freeze it to space with Fix or position it with constraints from Basic planes.

31. When creating external references or internal references be thoughtful of how they are affected by changes. Think; "how flexible is this reference?" It's not always easy and sometimes requires trial and error.

32. Profile sketches should be limited to lines and as few curves as necessary to describe the geometry.

33. Learn how to build a well named / organized tree and file system. It might seem trivial on small jobs, but on the big ones it becomes an absolute necessity.

34. When creating assemblies with several constraints, LABEL THEM so you know what you're looking at when one of them breaks or fails. Do it when you create the constraint.

35. Always comment actions/knowledgeware scripts/VB scripts so you know what you did.

36. Learn and understand Links

37. Learn and understand Parameters

38. Learn and understand PowerCopies

39. Learn When and Why to use Boolean Operations. They aren't always required, but they are OK to use when they are required. If you have to go out of your way to avoid them, then use them. KISS - Keep It Simple, S(illy)

40. Try to limit the number of items that you project or intersect into a sketch (use edges). If you do create use edges, make sure to select the item ONLY from the tree. If you select the item by picking the 3D geometry, the use edge will always use a BREP, which can be unstable on future updates.

41. Check and double check your CATSettings. Understand them.

1 comment:

  1. This blog is very nice for working.
    Catia is the advance software of any mechanical designing courses. this is the best step for career growth in mechanical field. according to me the best institute for Catia is EBEES.



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