Trimmed Sheet Tolerance Issue 1

[DHuskic]

Trimmed Sheet Tolerance Issue:
NX9 - Windows 7

We are receiving unusual results with this command and we can't seem to understand why. The curves are projected onto the face from a continuous end-to-end chain of curves.

When we use the Trimmed Sheet command on this patch, we get these splat-errors at a tolerance of 0.001.

When we change the tolerance to .0001, it works correctly. This tolerance change seems backwards though.

When we change the tolerance to .01, it appears to work correctly but cuts off the top portion of the sheet. The slice cut off at the top seems to correspond to the splats from the .001-tolerance. It also cuts off the bottom right hand and left hand portions.

Denis Huskic
Nx 8.5, 9
Windows 7

 

[JohnRBaker]

We'd have to have the actual part file before anyone could provide any sort of evaluation as to why this is happening.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[DHuskic]

The test part is attached.

Here is the general process (pardon me if I miss anything):
[ol 1]
[li]Open the part up in modeling[/li]
[li]Select Trimmed Sheet Command[/li]
[li]Target = Select the orange sheet body - Body (17)[/li]
[li]Boundary Objects = Select all the curves in the part, there should be 40[/li]
[li]Projection Direction = Normal to Face[/li]
[li]Region = Keep the inner patch[/li]
[li]Cycle through the different tolerances(.01, .001, .0001), and Show Result to replicate the problem above[/li]
[/ol]

Denis Huskic
Nx 8.5, 9
Kettering University Class of '17

 

[JohnRBaker]

OK, the loop of curves, all of which appear to be splines, some very small, were not created so that they are smooth as they transition from one curve to the next. I tried a couple of approaches to correct this. First I simply joined all the curves into a single continuous spline using the 'Join Curve' function. This way you get what you know will be a smooth curve. If I did this and then use this new single spline as the boundary it then works using either the 0.001 or 0.0001 modeling tolerance.

Th second approach would be to replace the 'corners' where there is a transition from one long spline to another long spline. I simply deleted the short little segments that made up the 'corners' and replaced them with 'Bridge Curves'. Again, if you do that the trim operations works for both the 0.001 and 0.0001 modeling tolerance.

Note that using a modeling tolerance of 0.01 appears to be problematic as it's just too large to assure a good result and should be avoided.

Also note that starting with NX 10.0, we've changed the default out-of-the-box modeling tolerances. For Metric parts this was changed from 0.0254 mm to 0.01 mm, and for Imperial parts, from 0.001 inches to 0.0004 inches. I went back to your original model and without making any changes whatsoever except for using the new default modeling tolerance of 0.0004 inches the trimming operation worked fine.

Anyway, that's what I've learned and you now have a couple of approaches that can be taken to overcome the issues that you've found with this model. But that being said, the real issues appears to be a less than ideal loop of curves being used as the trim boundary.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.