Buggy Surfaces

OGre_Cube

I made this surface using a revolve.  The profile used is that curve tangent to the inner circle.  It is just a section of a circle.  After making this surface,
 it does not behave properly.  The thicken, loft, sweep, and split features do not work on this surface.

S1mon

The surface isn't "buggy". You are asking NURBS surfaces to do something that they don't really like to do. You've managed to create an interesting degenerate surface. In general, when you revolve (or sweep) something, it's best to have the section normal to the path of the revolve. Typically you sketch the revolve axis in the same sketch or at least the same plane as the cross section you want to revolve. It's certainly possible to have the section at an angle, or even to revolve a 3D curve, but you need to be careful not to create situations like this. You are essentially creating the section at 90 degrees to where it wants to be.

Here's a model of something like what you did.

I created two configs: "fails" and "works". "Works" just barely works (e.g. it will only thicken in one direction), but it starts to show the issue. I added the Face curves to show how the surface is twisted and bunches up near the inner diameter.

Think of NURBS surfaces like a rectangular sheet of rubber or wire mesh. You can deform or stretch it a certain amount, but if you try to do too much, it may fail or cause downstream difficulties.

MichaelPascoe

To add to this:

Faces and surfaces that are a closed loop, like this face (or like a cylinder), must be split in two different locations. This is a current limitation due to the way Onshape handles surfaces.

So you could offset a line from your tangent line, so that there is a very small gap. This would allow it to work.

https://cad.onshape.com/documents/7c315baff9a32802372f04ee/w/f9b84c0b70daa134a57b22cc/e/447462fff2...

OGre_Cube

S1mon said:

The surface isn't "buggy". You are asking NURBS surfaces to do something that they don't really like to do. You've managed to create an interesting degenerate surface. In general, when you revolve (or sweep) something, it's best to have the section normal to the path of the revolve. Typically you sketch the revolve axis in the same sketch or at least the same plane as the cross section you want to revolve. It's certainly possible to have the section at an angle, or even to revolve a 3D curve, but you need to be careful not to create situations like this. You are essentially creating the section at 90 degrees to where it wants to be.

Here's a model of something like what you did.

I created two configs: "fails" and "works". "Works" just barely works (e.g. it will only thicken in one direction), but it starts to show the issue. I added the Face curves to show how the surface is twisted and bunches up near the inner diameter.

Think of NURBS surfaces like a rectangular sheet of rubber or wire mesh. You can deform or stretch it a certain amount, but if you try to do too much, it may fail or cause downstream difficulties.

The entire reason I am using a curve within a different plane is to have that specific curve on the face of a solid which will need to be cut with that surface.  I played around with it a little more.  I made an approximation using 25 or so lines and revolved that.  It resulted in something sort of looking like the face curves feature.  The approximated curve behaved much better.  to make it so it wasn't faceted, I then split it using a plane that contained my axis and made a second approximation using the spline tool with the edges of that split surface.  This got me close enough that I was able to use my surface normally.  I wish it worked how I initially tried so it isn't an approximation, but I see how it would be difficult to implement.  I think solidworks might be able to do what I ask, it seems to grunt it's way through things.

EvanReese

This looks like a problem that may have a better approach. Can you explain more about the goal? It looks like your goal surfaces are just a planar circle with a hole in the middle. Is that right, or are they slightly conical? Either way, I think there'a cleaner method.

As for Solidworks, you might be right, but fundamentally Solidworks and Onshape, (Creo too, I think) are built on the capability of the Parasolid 3D kernel, and therefore they share may off the same challenges, limitations, and workarounds.

steve_shubin

Upon reading Evans post, I thought I’d give it a try with flat discs

Now, if the discs had some kind of a curve on the surface, well right now, I don’t think it would be much different once you came up with your disc shape

At least in this case there’s not much to it.

And I’m sure somebody could find a way to shave down the amount of features or the amount of steps

https://cad.onshape.com/documents/d1a98606e25278085ca72d0d/w/fdf966ee8352ea13f91fdaaf/e/584b327585088590766df952

steve_shubin

Added 2 more Part Studios and a new link in the post above, to a document that now has flat discs, bulged or pillowed discs, and bulged everything 

OGre_Cube

Evan_Reese said:

This looks like a problem that may have a better approach. Can you explain more about the goal? It looks like your goal surfaces are just a planar circle with a hole in the middle. Is that right, or are they slightly conical? Either way, I think there'a cleaner method.

As for Solidworks, you might be right, but fundamentally Solidworks and Onshape, (Creo too, I think) are built on the capability of the Parasolid 3D kernel, and therefore they share may off the same challenges, limitations, and workarounds.

as you can see the disc follows a "line" on the the curved surface of the "cube"  I can get close enough by remaking an approximation with a spline, I just wanted to use an exact curve since this is cad and not me with a hacksaw in the garage.

EvanReese

If you're willing to share a link to your doc, I can get in there and take a crack at it.