6 Replies Latest reply on Sep 18, 2013 6:54 AM by Dave Krum

    cannot get 2d .dxf to extrude in SW (geometric condition error)

    Dave Krum

      Hi All,

      I'm having an issue with trying to get a 2d sketch (.dxf) from Autocad extruded in SW2010.  I did check on this forum for some past related threads concerning this and have tried some of the responses, but still cannot get it to extrude.  I'm getting the common "cannot perform the extrude feature due to geometric conditions".  I must have overlapping lines or lines not extended / intersecting somewhere (but not sure where).  This is always a pain when trying to burn something like this in my flamecut software and appears to be the same in SW.  Is there something in SW that will check and show me WHERE the problem area is on the sketch so I can zoom in and fix it?  I can successfully extrude the perimeter to a solid with no cutouts but when I select the whole thing in the contour box to put the cutouts in the shape, I get the error.  See attached screenshots.  I've also attached the .sldprt.  Thanks!

        • Re: cannot get 2d .dxf to extrude in SW (geometric condition error)
          Jim Wilkinson

          Hi Dave,

           

          Try using Tools, Sketch Tools, Check Sketch for Feature.

          http://help.solidworks.com/2014/English/solidworks/sldworks/hidd_sketch_diagnostics.htm

          You will have to use it multiple times to get rid of the 4 problems.

           

          There are two places with duplicate, overlapping arcs (on the two D's) that need to be deleted.

          There are also two places where a line and an arc intersect one another because they aren't perfectly tangent (bottom of center C and top of small R). Those are easily fixed by just making the line and arc tangent on each of them.

           

          I hope this helps,

          Jim

            • Re: cannot get 2d .dxf to extrude in SW (geometric condition error)
              Dave Krum

              Thanks for the info Jim.  I've fixed all of the issues except fort the one you mention at the bottom of the center "C".  I can't see any intersecting lines.  Unfortunately, I have software OpenGL enabled and cannot disable it apparently because I now my junkie integrated graphics card running SW.  My Quadro was taken out for replacement which I don't have yet.  With OpenGL enabled, I cannot zoom into problem spots from what SW is telling me.

                • Re: cannot get 2d .dxf to extrude in SW (geometric condition error)
                  Dave Krum

                  Did actually get it working by using the tangent relation as suggested.  But without the tip of where to look, and without the zooming capability due to openGL being enabled, I wouldn't have been able to find the issues.  Thanks for the help!

                    • Re: cannot get 2d .dxf to extrude in SW (geometric condition error)
                      Jim Wilkinson

                      Hi Dave,

                       

                      There are actually two tools at work here. There is Check Sketch for Feature and then sometimes it will give a message asking if you want to try to repair it. If you hit OK, it will go into the Sketch Repair tool. I get some sort of zooming problem where all the geometry disappears if I hit OK and go into the Sketch Repair tool. But, if you are in that tool and turn off the magnifying glass and then do a zoom to fit, instead of trying to zoom in on the problem, it gives little yellow circles around the problem areas. This is how I found the two overlapping arcs. Actually, if when you use Check Sketch for Feature and then hit cancel (so it doesn't go into Sketch Repair), it will highlight one of the bad arcs. Hit delete to get rid of it. Then hit check again and repeat to get rid of the other one. Once you delete those two arcs, then run Check Sketch for Feature again and it will report one of the self intersecting cases and select the line that is causing the self intersection. I can't see the overlap by zooming in either, but I figured it must be where the line and arc meet because the other endpoint is a line coming into a line so they can't overlap. I added the tangent to fix that. Then I ran Check Sketch for Feature again and it highlighted the arc on the R being overlapping. Inspecting that one, again, I couldn't see an overlap, but due to the angle that the arc and line come together at the tot, I figured it had to be there and not at the bottom.

                       

                      So, In this case, the Check Sketch for Feature tool does a fairly good job of reporting and highlighting the entities involved. The Sketch Repair tool isn't really designed to handle these exact cases well and hence why it was not of as much use.

                       

                      I hope this helps in troubleshooting in the future,

                      Jim

                • Re: cannot get 2d .dxf to extrude in SW (geometric condition error)
                  John Sutherland

                  In your situation I would:-

                   

                  In System Options>Sketch, check Display entity points in sketches. 

                   

                  Employ Select Chain to identify closed profiles.

                   

                  Employ Select Other to reveal coincident elements which can then be deleted or altered.  Inexplicable (entity) points on lines are clues to an underlying element.

                   

                  Salvage incomplete profiles by "tracing" them (Convert Entities) to a new sketch.

                  • Re: cannot get 2d .dxf to extrude in SW (geometric condition error)
                    Dave Krum

                    Thanks for all of the help guys!  Much appreciated