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MohaSharifi10-Marble
10-Marble
January 13, 2017
Solved

Problem in creating section in drawing

  • January 13, 2017
  • 5 replies
  • 13588 views

I want to create a cross section from an assembly in drawing, but following error is appear and no cross section is created, can anyone help?

 

Cross-isecition creation in view "new_view_10", on sheet 1, aborted.

Best answer by BobSchwerdlin

There are times when Pro/E, WF and Creo cannot properly create an X-Section.  In my 20+ years of using the program 8 hours a day, I have never been able to understand why this happens, but can offer a solution.  Instead of making the X-Section directly on (for example) the RIGHT datum plane, make a datum plane that is 0.001" (0.025mm) offset from the RIGHT datum plane and place the X-Section on the new plane.  It should work perfectly.

Bob Schwerdlin

Dukane Corp.

5 replies

B
BobSchwerdlin1-VisitorAnswer
1-Visitor
January 13, 2017

There are times when Pro/E, WF and Creo cannot properly create an X-Section.  In my 20+ years of using the program 8 hours a day, I have never been able to understand why this happens, but can offer a solution.  Instead of making the X-Section directly on (for example) the RIGHT datum plane, make a datum plane that is 0.001" (0.025mm) offset from the RIGHT datum plane and place the X-Section on the new plane.  It should work perfectly.

Bob Schwerdlin

Dukane Corp.

StephenW
StephenW23-Emerald III
23-Emerald III
January 13, 2017

I have this problem on occasion. It seems to have something to do with intersecting a small edge or surface but I don't really know why.

My usual solution is to offset the x-section just a little amount, maybe something as small as .005 inches. Usually I run in to this problem on large assembly drawings so I am not dimensioning much but if you are dimensioning across the x-section, this is likely an unacceptable solution.

I think I have also fixed it with a accuracy change in the assembly but you need to be really careful with this as it can cause other issues depending on your model.

Chris3
Chris321-Topaz I
21-Topaz I
January 13, 2017

It is because the math for drawing intersecting geometry is very difficult. If you remove all overlapping geometry, increase the accuracy or simply change the cross section so that it is either offset (as mentioned above) or change the visibility to exclude any areas that have small surfaces this issue will likely go away.

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mender12-Amethyst
12-Amethyst
January 13, 2017

Confirming what others have said, and explaining a bit further:  when showing an xsec in a drawing, we have to perform a cut, making cut geometry, because we need to be able to make stable references to the edges made by the xsec operation.  This operation can fail for much the same reasons as an extruded cut with the same effect could.  This is also the reason that putting an xsec view in your drawing can mark the solid as modified (having made new edge ids by performing the xsection, we need to store them if we are to have stable references).

In assembly mode, we can visualize the cross-section by quicker methods, 'draw the assembly but don't go past this plane' plus figuring the contour of the cut surface.

    M
    MohaSharifi10-MarbleAuthor
    10-Marble
    January 14, 2017

    Thank you all for your helpful comments. Your explanation helped me to find the problem. First I offset the section plane and then modified the geometry a little at the section plane then the problem resolved.

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