I embarked on my first modelling session with SC 2011+ yesterday, and my experience was very discouraging.  I'm attempting to add chamfers (variable setback) to a solid, which is an extruded set of splines.  The chamfers need to meet at the midpoint (or midplane) of the modified edges.  In other words, if the solid is 2mm thick, the chamfer setback on the 2mm face is 1mm.

See pic - I'm adding the chamfers to 2 co-planer edges that meet at a vertex, and the 2 opposite edges.  The pic shows 1 solid in 2 views.  I created this via the workaround below.

The first chamfer works.  The second chamfer usually works.  Sometimes the third chamfer works, but I entounter failure as follows:

1.  Pull, Up To successful chamfer - FAIL

2.  Pull, arbitrary value, edit properties to match successful chamfer - FAIL

3.  Pull, arbirtrary value, Pull again to enter set-back values - FAIL.

Furthermore, my attempts a workaround have been troublesome.  I figure I could Pull half of the needed chamfers and proceed with mirror and/or patterns:

4.  Select new edges created by chamfer, select plane (to use as mirror plane) - FAIL (cannot define a plane from the coplaner chamfer edges).

5. Manually create mirror plane, mirror chamfer faces, trim (i.e. Combine) appropriately, then create a radial pattern with Move of the faces - FAIL (either creates a faulty pattern that does not respond to count/degree editing, or doesn't create a pattern).  Using solids as a pattern members was successful - SC had a hard time with the spline faces.  I did try this with Face>Properties>Chamfer>True and False.

In general is seems that SC has a major problem with chamfers on spline edges.  Not good news for me, since this describes almost all of my modelling needs.  Hopefully I'm doing something wrong.

 

Two vids showing more spline-defined solid problems:

 

http://www.screencast.com/t/xTdETg0t

 

http://www.screencast.com/t/J4XegbvwV

 

 

Geometry errors are one of the main reasons why the bodies do not merge. I was able to merge the bodies together. See link:

 http://screencast.com/t/Motubo0YIjAq

Best Regards,

Vimal

Vimal, I see that you've defined your plane via 3 points.  Is that the only difference?  Have you 'Simplified' this solid before you performed the mirror?  Certainly the method of defining the split/mirror plane should not impact the success of an error-free split and subsequent mirror/merge.

Why does SC generate error-laden solids to begin with?  If this was imported geometry, I would completely understand.  But this is native geometey created from 3 curves and 3 pulls, which is then split about a mid-plane defined by 2 opposing, parallel faces:

screencast.com/t/UQK6bA1loQP

 Yes, defining the plane using 3 points makes the difference. Selecting 2 faces and creating a plane, generates a plane midway between the faces. Since this geometry is uneven with a lot of spline faces, i would recommend defining a plane by selecting points. In your case splitting the solid using the plane you generated created a non manifold geometry which can be seen while perfoming a geometry check. The model I used in my video was created from scratch with no repair tools being used.

Best Regards,

Vimal

 Interesting - thanks for the workaround.

 Ideally, SC (or any CAD program) should create 2 error-free solids when split by any plane that intersects the solid.

 

I don't know what non-manifold geometry is, but in principle, if the solid is 3mm thick, and the setback of the chamfers are 1.5mm, then the following three planes SHOULD be identical and successful:

1.  Plane defined by selecting parallel faces which are 3mm apart (this is, the midplane of the solid).

2.  Plane created be selecting one (or both) of the chamfered spline edges (the edges that lie on the curved surfaces of the solid).

3.  Plane created by selecting three points on the edges mentioned in #2 or at the vertices of these edges (Vimal's approach).

Hi Patriqq, cutting a solid in a plane that is 'parallel' to a plane defined by splines will fail in most CAD systems I have seen. This is because of the splines being a bit imprecise and like to 'swing' between their defined points, so they will not be precisely on that plane if looked at real close. A cut or mirror will create minute debris faces, gaps or overlaps. Programs like Rhino work around this by using less precision or higher tolerances, though that'll fall onto your feet once you import this into more precise systems. If you want to create a solid that is going to be mirrored, I'd recommend creating the mirror plane first, then build the solid on that. This way, you will eliminate tolerances that will cause trouble downstreams. Also, you could 'overbuild' you solid, that is not stop at the mirror plane, and use the mirror plane to first cut, then mirror. This is both good practice no matter what system you use.

 

martin kopplow:

... use the mirror plane to first cut, then mirror.

 This is exactly what I was attempting.  I do appreciate the perspective, comparing SpaceClaim to other CAD programs.  I reproduced some of my modelling attempts on Autodesk Inventor this weekend, and met many of the same problems.

"First cut, then mirror" requires the solid to be overbuild over the plane, so you can slice off a full slice of it and thereby making sure there is a defined plane to be used for the mirror.

I've revisited Inventor and Solid Edge and found that they can chamfer spline edges correctly and without issue.  Apparently I was missing some steps at my first attempt.  Currently this issue is filed as a bug report with SpaceClaim; I would like to see them solve the issue.

Meanwhile, I've found that the best workaround for SpaceClaim is to copy my original, extruded solid and apply one chamfer per solid.  Then I superimpose (move) and combine/delete such that my desired solid remains.

This approach avoids the corruption of the edge that was occuring in my original approach.