I have a problem with making a thread for screw like part which is attached bellow.
And I can't find appropriate answer anywhere.
I have a problem with making a thread for screw like part which is attached bellow.
And I can't find appropriate answer anywhere.
Marko,.. it needs some help, a guide curve and you will need to clean up the spacing of the profile or the path so it does not run into itself..
I actually found easy way by my self that works with no problems (I believe for any type of thread):
Divide sketch that should be swept-cut in two pieces. Problem was because it should look like continuous curved thread, and there was a problem with "zero-thickness". So idea is to divide it in two sketches and thus two swept-cuts, one for convex part, and one for concave part.
I work with threads every day and have found that threads like this (we call them rope threads) can be difficult to model without either errors or incorrect geometry. I will keep your solution in mind for the future. Thanks!
Don't know if this might work the same for SW as it did for Pro/E, but I found the most robust was was to create the helical cur as a surface, then use the surface to remove material. A surface (in Pro/E anyways) didn't care if it overlapped itself. Might be a cleaner way....
Now, where did I hear that before.....
btw,.. the image I show was to illustrated the overlap and get the error (since Marko was using a solid)... the file I provided is a surface.. it does not work either (although there are workarounds to make it work).
Pro/e's kernel is more tolerable,.. I miss it too.
Hi Marko,
Might be nice to know that 2016 has now got this as a standard feature.
You can edit the file it's generated from, and add new threads etc, very overdue.
That is supposing you are brave enough to run 2016
Hi Marko,
Nice solution you found. You are correct, the sweep is running into a zero thickness condition due to the equal pitch and profile heights. As Matt points out, you can easily create threads in 2016 using the new Thread command. I've taken your profile, split it in two (as you did), created Library Feature Parts out of them (this is what Thread uses for Profiles much like Structural Members), and created your threaded body.
I've attached the model and profiles for you if you (or anyone else) happen to have 2016.
Out of curiosity, what are you making with this type of thread on it?
Is there anything else aside from the profile that you add to the part to finish the thread?
Jody
I actually found easy way by my self that works with no problems (I believe for any type of thread):
Divide sketch that should be swept-cut in two pieces. Problem was because it should look like continuous curved thread, and there was a problem with "zero-thickness". So idea is to divide it in two sketches and thus two swept-cuts, one for convex part, and one for concave part.