Draft Splits

chris_sturgis

I  have previously talked to someone in support about this but I dont remember if anything came of it. I also dont think it was well understood what I need, and I have a good example to use now.

So my issue is with the draft tool, specifically that you can only add draft in a single direction. I am currently working on a simple squeegee model, see below. The Blue line represents my desired parting line for molding this part, it also represents the front plane of the part studio.


 If I want to draft this part for this parting line I can go into the draft tool, select the front plane as my neutral plane, select all the face I want to draft, then select my draft direction.In Onshape I can select one of two draft directions, basically I can make a V shaped part or an A shaped part.


I want more of a diamond shaped part, a combination of the two available draft angles, where the draft angles inward from the neutral plane on either side. In other software you can split the draft direction at the neutral plane in order to accomplish this. This is something that Onshape needs to add quickly.

bradley_sauln

Before performing the draft you can use that same plane to either split the part or just the faces you are trying to do a split draft on and then perform drafts on either side. Not ideal but if you are trying to get something finished it will work.

grochino

Hi Chris, I believe I was the support person who corresponded with you on this. I still have you tied to the improvement request for a parting line draft option, but thank you for providing a good example for this. I will add this information to the request. Thank you again for the feedback!

NeilCooke

There is also a custom feature that does this: https://cad.onshape.com/documents/578ceef1e4b01a7c3b1f353f/w/fa319c720c94a559de053612/e/2d4015dbb936ea708337450a

matthew_stacy

@chris_sturgis & @bradley_sauln, I must say that I find it less than intuitive that the NEUTRAL PLANE option of the DRAFT tool doesn't symmetricly draft a part (or selected faces thereof) about the selected NEUTRAL PLANE.

In effect the only parameter that Onshape actually harvests from the plane selection is the direction of pull. I could select any parallel plane and achieve exactly the same result.  What is the use case or application for Onshape's neutral plane drafting?

It looks like split face/s > parting line draft is the only useful workflow to draft parts for mold release.

matthew_stacy

S1mon

If you were to take a cross section where the drafted surfaces intersect the neutral plane the section would be the same before or after draft. That is where the draft hinges. That's why it's called the neutral plane.

9 times out of 10 I use parting line draft. Neutral plane draft is more simple to implement, and many CAD tools have had that before they added parting line (or "curve driven") draft capabilities. Typically the only time I use neutral plane draft now is if the only edges I have for a surface are curved and I want to keep the resulting drafted surface a plane, just tilted.