2020 Solid Sweep Issue

[davidXH49F]

I was really hoping 2020's solid sweep would work for my application.  It seems that its really hit or miss and may depend on the "curviness" of the path.  Can someone take a look at the attached file?  

Basically, this is a ball end mill that needs to stay vertical and be swept along the "toolpath" the way a normal 3 axis milling machine would cut it out.  I'm going to use the solid as a subtraction tool later in my design.  I just need to sweep this solid along this path...

Thanks,

David.

[johnsonshiue]

Hi! Indeed, Solid Sweep can feel flaky at times since the geometry is probably the most complicated and compute-intense in Inventor. There are fail cases for sure. In your case, you select parallel option along a 3D spline path. I will need to take a closer look. So far, it looks like a bug to me. If the bottom of the tool is flat, instead of round, does it work?

Many thanks!

[davidXH49F]

Thanks for looking into it.  I do these sweeps an average of once a week (automotive hose industry) and have always had trouble using profiles and "path guide and surface" on the more curvy paths.   I was really hoping that 2020 solid sweep would take care of this issue, because the final shape is simply the result as if a ball end mill moved along the path (staying vertical) and cut everything in that process.

I did try it flat on the bottom and also could not get it to work.  I've tried it a lot of ways actually.  Simple, straighter paths do work and it is great.

David.

[johnsonshiue]

Hi David,

I took a quick look at the part. I think there are multiple issues here. The regular Profile Sweep does not work either. I believe it has something to do with the path. The path seems to have tangency discontinuity. Does the path have to be precision? Can it be tweaked or replaced with a spline?

Many thanks!

[davidXH49F]

Thanks, I'll look into the tangency thing.  Our customer designs in another CAD system and gives us a drawing table with the points and bend radii for the sweep path so we can design the tooling.  These points are rounded off to only 2 decimal places.  On this one, it looks like several of the points are supposed to be co-linear, so that's where you noticed the tangency issue.  I'll eliminate those extra (nearly colinear) points and try again.

Interestingly, that path, as it is, will sweep just fine for very simple geometry like a circle.   See attached.  

I'm hoping this has been my issue all along!

Thanks,

David.

[davidXH49F]

It was a good thought, but I just fixed the non tangency issue and it still doesn't work.  See attached.

[WHolzwarth]

Well, Solid Sweep still has lots of issues, far away from being perfect. Here's a workaround for this basic task, but it failed in combining both resulting bodies the easy way.

That's the worse news. Better news: Lots of UI changes, and blue icons all around.

I'm wondering myself, if I'd really would have needed that.

[davidXH49F]

Thanks, I really like your workaround (and may use it in the future), but you ended in the same place that I did with my own workaround--the boolean operations fail... 

Here's my workaround--I performed a solid sweep on a sphere, then projected the 3d sketch down the vertical axis to a plane.  I offset that projection by the radius of the sphere (both directions) and closed the loop with some lines.  I then extruded it upwards, and trimmed it using a surface that I made from the 3D sketch.  The geometry ended up being very similar to yours, but the edges are too close (yet not perfect) for boolean operations.  I ended up having to make larger differences in the edges (increased my offsets by 0.005 inch) to get boolean operations to work, but the result is ugly.

David.

[johnsonshiue]

Hi! This is a very interesting case. I took a closer look. The difficulty is indeed related to the path. Interestingly, if there are no arcs, the solid sweep actually succeeds. I guess this has something to do with the transition geometry. Regardless, it should work.

I managed to find a workaround using a sphere solid sweep and ruled surface. You can see the surface in the middle overlapping. I think this is why solid sweep fails. I will work with the project team to understand the failure better.

Many thanks!

[davidXH49F]

Thanks Johnson.  I looked at your file and noticed that there is an overlap in the ruled surface that you created.  A split/trim isn't going to work with that surface as is. 

See attached.  Previous to 2020, I had the same issues with these types of paths using sweep (using a guide surface to keep it vertical).  A regular unconstrained sweep would work, but the profile would twist, which creates geometry that isn't functional in the real world for several reasons.

Thanks so much for looking into it, but so far the workarounds don't actually work (boolean operations fail, split/trim fails, etc).

My workaround has been to sweep the segments of the path that work and loft the portion that won't sweep.  It looks clean, but its not very accurate geometry.

David.

[johnsonshiue · Accepted solution]

Hi David,

Houston, we have a solution here. Please see attached file. Instead of using the cylindrical rod (with rounded end), I used a ball to sweep along the path. Then sweep the solid vertically. It should be very close to the real solution if not 100%. Think about it, the rod is indeed like a sweep along a straight path. I just to it in a different order.

Certainly, the original case should work. But, at least there is a solution only available on 2020 and later.

Many thanks!

[davidXH49F]

Awesome!  Thanks!  Such a simple workaround.  I wish I had thought to use Solid Sweep twice!

[Anonymous]

well done!

tricky but works...

[johnsonshiue]

Hi! @davidXH49F, @Anonymous, and @WHolzwarth,

I am revisiting this case. Actually the Solid Sweep does work without much creative workaround. It seems that the planar face at the bottom of the cylinder can be an issue. I added a fillet to make it a half sphere. Then Solid Sweep simply works. Please take a look at attached part saved in 2020.4.

Many thanks!