Bolts - threads or dashes?

[automaton2]

I am an entry-level engineering student.
As I started learning PTC Pro Engineer 5, I ran into a problem. I asked a person with a major in drafting about this and he couldn't answer my question.

Do I need to draw threads on every bolt I am designing in Pro E? What is the easiest way to do this?

If not, than my hole for a bolt is geometrically narrower than the bolt so there is no way I can stick an unthreaded bolt in to a smooth bore without causing geometric interference glitches.

How would I solve this problem in Pro Engineer 5?

Thank you for your time.
V.T.

 

[jebaileyjr]

What youll find is that companies do it both ways. I have been at several companies doing design work, and some require you model all threads and some require you model some threads. Where I currently work, you only model non-standard treads and all standard threads are done as cosmetic. This goes out the window when you need a rapid protoype with the threads processed during the rapid prototyping and not as a secodnary operation.


If you have to model, you do a helical sweep (sorry if I am assuming you do not know this). The helical sweep will not always prevent interference check problems unless you constrain the bolt to all degrees of freedom so that the bolt thread start matches the hole thread start.





Jim

 

[automaton2]

I know what helical sweep is. There is no better way to do threads in Pro E?

What if I accidentally start my internal and external helical sweeps at different angles...
Well...
My plans are for educational purposes so there is not going to be a finite element analysis performed.

Do I make smaller holes or narrower bolts to compensate for the threads?

 

[automaton2]

Thank you, jebaileyjr.

 

[jraquet]

If you have mating parts, the angles need to be the same for both sweeps, or you will have a different thread pitch.


Your bolts can be narrower if you will add threads or thicker if you will cut threads, vice-versa for holes (smaller to cut, larger to add)

 

[dr_gallup]

Unless you are making RP models or molds from your parts it is silly to explicitly model threads. Use the cosmetic thread feature.

 

[Mindripper]

As dr_gallupand jraquet aresuggesting, the use of modeled threads will bog down your computer with needless detail, and they are a lot more work. For threaded holes, use the Hole Tool in Pro/E. For male threads, you have to look up the specsfor the major and minordiameter. If you are intererested in the details of schematic screw thread representation, see ASME Y14.6 - 2001.


Be very careful when using the interference checking utility available in most CAD packages. While they can be useful,they will flag things like fasteners - and not flag things like features that are nominally very close, but could interfere when the tolerance is applied to one part or another. I rarely use these interference checkers:they are nota substitute for good design practices and properly detailed drawings.

 

[automaton2]

thank you for your advice

i will try to get a hold of
ASME Y14.6 - 2001
by the use of my engineering friends

 

[AaronMejia]

Over here we create the screw with the total diameter and then we do a helical cut to create the thread. However, the use of threaded screws is forbidden for design and it's only used when you need a drawing for quotation of the screw or something like that. Instead, we create a simplified rep of the screw without threads, dents and/or slots and that's what we use in our assemblies. Having all those details in a screw that you use 200 times in an assembly can surely use up a lot of memory. I had a case of an assembly with screws using all their features and, by using the simplified rep instead of the master rep, we reduced the memory consumption from 1.2 GB to about 480 MB.