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Representation of threads and tappings of an assembly in drawings.
Olivier_T_Prof_Si
Member Posts: 8 EDU
I'm desperately trying to correctly represent the threaded and tapped elements of an assembly.
I have used the drilling and external threading functions in my document. (I'v also tried Threadcreator et threadlab but there is no correct representation on the drawings).
I get a good representation of the individual parts. But if I represent a cross-sectional view of the assembly, the threaded / tapped areas overlap. The hatching of the bore should stop at the shaft contours.
Am I doing something wrong? Is there a way to represent these threads / taps correctly?
See drawing tab
https://cad.onshape.com/documents/2f502b9cc71738081a3675db/w/7115f02d0c559304a03ec7b2/e/1bcac897a4a6c4b5fafb063d
Answers
I think if you right click on the view, show and hide, screw threads.
@Ste_Wilson this is not exactly what I want.
the hatch lines of the bore #6 should not be visible in hatched zone of #7.
I expect this :
@Olivier_T_Prof_Si
You have pretty severe interferences in your assembly here:
Try this… Right click on the assembly view and select Show/hide…. Show part intersections. Drawing views do not automatically process part intersections from interferences. It would slow down every drawing view creation if we did, for what amounts to a very small number of views where this matters.
These intersections seem normal to me, since these interference zones are threaded parts. Unless I've defined them incorrectly...
When I right-click in the assembly, and select Show Part intersections, nothing happens.
If I activate the shaded view, I do have the male parts in the foreground. Although the hatching continues to cross
@Olivier_T_Prof_Si,
As a workaround - have you considered doing a "duplicating/copy workspace" of the model and cutting 3d threads, and using this model only for detailed section views - and original model for regular drawings (showing simplified threads)? This is more work, but would yield nice results. I have modeled taps and dies for cutting 3d- threads in standard sizes, (these are derived and boolean cut into part), I would share, but it looks like your threads are for optical equipment - and I'm sure those are unique sizes. You might want to create your own library of these, if you have a future need.
I do agree that the "drawings" need improvement in this area.
Don't copy the workspace for something like this! You could use a configuration that either has modeled threads or use "move face" to remove the interference and use that in the section view.
I was hoping using the "show part intersection" options would let you select the hatch regions separately but that doesn't seem to be the case unfortunately… That would be a good improvement request…
There's a "hack" where you could change the hatch style of the internal nut part to be either solid or much denser so it hides the other one but not an elegant solution…
Thank you for both your responses.
@rick_randall
I design optical equipment. I often use threads that are not in the Onshape database...
Using the configs allows you to quickly see the different threading possibilities in the drawings. None of them is really satisfactory, but it helps you to see more clearly and choose the most suitable method later on.
Thanks @eric_pesty for the hack. I've also had this idea, and it works, but isn't very elegant. Putting hatchings of the same style, and same inclination and playing with the scale factor, it can give the illusion. But some continuous lines should be removed from the interference zone, and it's not possibible to remove just a part of such a line.
If the hatch style could have a background color set to white, that might solve my problem ;)
@Olivier_T_Prof_Si Here is one example of metric 3d thread cores (for internal through hole, through a plate) - copy and modify to suit (if you think it would be useful). To use just derive, position, and boolean cut, it's a pretty quick operation. And I do agree with you about creating configs. instead of extra part files. Just food for thought.
https://cad.onshape.com/documents/e62d348b7b75d31ef2575a5e/w/9fd2841fad77cad9457784e6/e/ffbdfb3f92eb6195fbdbcf10
And I have other similar part tools for cutting external threads But I think you get the idea. It's the concept I'm trying to show here.
Thanks for your tips and doc sharing @rick_randall
I often use the feature ThreadCreator to cut internal or external threads. Pitch, ø, and shape, can be adjusted as you want.
https://cad.onshape.com/documents/6b640a407d78066bd5e41c7a/w/4693805578a72f40ebfb4ea3/e/f8aea9e5c33e02eab0854a4f#_ga=2.61103343.279186957.1726994362-746991051.1726994362
What I need most with my students is to have correct representations, even if the diameters are outside the standards.
If I have manufacturing needs, then we adapt, and do everything “by hand” with a method similar to the one you showed me.