Part of solid disappears when using draft

[natemclain]

I'm trying to add 2 degrees draft to some parts for a mold.

When I select the parting plane and the solid it displays properly but the portion of the model disappears.

Really strange, I can't find it on any component in the model.

I have attached some pictures as I can't share the model.

Has anyone seen this behavior?

[TheCADWhisperer]

File>Export and then Attach your *.f3d file here.

[wmhazzard]

Does it happen on all of the parts or just the center one?

[natemclain]

All 5 act the same way.

If I select the top of the cylinder and make the draft larger at the bottom it works fine, but thats not what I need. 🙂

I'm at the point of trying to reduce the diameter of those 5 cylinders the amount of the draft and then add draft to make the bottom come out right.

Seems silly but software is screwy sometimes.

Its one of my biggest complaints about Fusion 360, draft, parting line draft, and draft for lettering for molding & pattern making purposes.

[natemclain]

Ok I exported the one piece with the issue to see if you'll can duplicate the same issue as I.

[natemclain]

I attached the .f3D file to the main thread.

Thank you for your help!

[laughingcreek]

this version seems to work, probably b/c you parted it into 2 halves.  I don't think it could figure out how to heal the geometry as it went around the bottom side of the tubes.  does create an overhang though.  might be ok if these are sprues.

[natemclain]

The draft angle needs to start at the bottom and get smaller at the top.

Looks like you selected the top of the cylinder and made it bigger at the bottom which creates the overhang, that won't work. :-), I was able to do the same thing you have. If you select the parting line or the XY origin plane with 2 degrees draft you will see what I mean. I'm not sure if yours will disappear like mine or not.

Looks like I might have to go back to reducing the cylinder by the amount of the draft and then draft from the top of the cylinder so there is no overhang at the bottom.

[natemclain]

Well looks like I'm going to have to delete the existing solid cylinders that stick up and create new ones and join them to the main body with draft. Hopefully someone has some insight as to what is going on and why Fusion can't add draft without barf'n on itself... Seems like a simple task without the fillets that were previously there, I removed them to help get the draft feature to work. No dice...

[wmhazzard]

I offset the faces by a minus .001" so .002" smaller in diameter and was able to draft the parts the way that you want. I don't know if that would be acceptable to your model but it might work. 

[natemclain]

Very interesting... definitely within the scope & tolerance. So that’s an ok solution.

i was also able to delete the cylinders and create them smaller and add draft with the push/pull tool and have it come out right.

thank you for mentioning the offset with the small amount as I hadn’t tried that.

i hope Autodesk keeps working on changing and improving the draft & mold maker features in Fusion. It’s definitely needed. We don’t all work in the world of straight lines and 2D geometry, which Fusion works really well in that environment. We need sophisticated drafting and mold/pattern making feature sets.

Woth that being said what is the best mold / pattern making software out there?

ive used Spaceclaim and it performed really well. I might have to go back to it...

[wmhazzard]

I do some patternmaking and mold design as well and draft can be challenging, sometimes you just have to beat it into submission. 

[TrippyLighting]

Look at the attached model. Change the angle that I am pointing to and see what changes.

Then please explain how drafting works and why it does not in this case.

Hint: The picture alone can already explain that.

[wmhazzard]

@TrippyLighting I do not know what you mean but there is clearly something wrong, possibly a bug, with the draft command. The drafts fail when the bottom cylinder is split in half. When that is done, the top cylinder cannot have draft where the top is smaller, only larger. If I offset the bottom face by .002" I can get a successful draft, if I only offset the face by .001" I get a strange body on the bottom and the top disappears. Something seems to be off when the intersection of the top cylinder is coincident with the bottom face. Also the floating box that you can type the angle into is missing on my screen. 

[TrippyLighting]

Cool test! I had not thought of that.

I think "the truth" in what is a real draft is somewhere between the geometry created by my file and by your file.

Both can be considered valid.

If you change the draft angle on both of our designs to something much steeper you can see the difference in geometry. 

In your file the cone still is extruded from the base circle and intersects the horizontal cylinder, so in essence the surfaces of the cylinder and cone are not tangential.

In my file the cone surface will always be tangential to the horizontal cylinder (or so I think ).

The question is what would one consider to be the correct geometry ?

Both likely achieve the same goal and if you put a chord fillet on yours it'll look better.

[wmhazzard]

Technically your model would be correct in the real world. If you notched a piece of tapered tubing, you would get a cut like your model. That is the problem with the draft command, just picking a center plane may not be the correct thing to do in may applications.

I don't know what the OP's intent is but if that is a core and he needs draft for the core prints, I would draw it up like this instead, with the draft starting at the top of the horizontal tube. 

[TheCADWhisperer]

---

@natemclain wrote:

....We need sophisticated drafting and mold/pattern making feature sets.

With that being said what is the best mold / pattern making software out there?

---

I wouldn't attempt to judge "best out there", but several years ago Autodesk purchased MoldFlow and incorporated the mold design tools within AutoDesk Inventor Professional.

By the way - I would have modeled your part very differently than you did. 

[natemclain]

The intent was to use the solid that was created in Solidworks by a customer and add all the draft angles for a core assembly. When the core was split and draft was added using the parting line plane Fusion didn't like it for some reason. The cylinder that needed 2 degrees draft added is part of the internal area of the casting. The core print hadn't been added yet.

I have attached an example of what I was trying to accomplish at the time.

I was able to work through the issue, it was just puzzling why part of my solid model was actually disappearing completely when I used the draft tool.

I'm not sure if anyone was able to duplicate that behavior from the file I exported and attached to the thread. Perhaps it has something to do with the way Fusion imported the sldprt file and the problem might not exist on the F3D file I exported for the forum.

It's still bizarre behavior and seems like it should work just fine.

I'm also experiencing some strange issues with fillets now, all these little issues turn into allot of wasted time and frustration that isn't productive to the task at hand. 🙂

It just seems silly.