4 Replies Latest reply on Nov 16, 2017 1:19 PM by Tyler D.

    Help repairing sketch

    Tyler D.

      I'm hoping for some help, I'm stumped with this.  To describe how I made this initially: I had an enclosure, with draft, no cutouts in the sidewall.  In the assembly, I made a reference plane to indicate the lowest face of the PCB (with the narrowest dimensions due to draft).  This ref plane was below the parts and mate in the assembly feature tree if that matters.  I did an Insert Component > New Part for the PCB, then the part sketch was on the ref plane and made by the Intersection Curve with the inner faces of the enclosure side wall.  This gave me the outline of the void within the enclosure at the level of the PCB.  I then used this outline, did an Offset Entities 3mm to leave a gap, and ticked the Construction Geometry: Base Geometry box to give me the desired outline of the PCB board.  Extruded to desired thickness, everything was good.

       

      After adding some cutouts through the sidewall of the enclosure and some ribs for a captured nut, my PCB part (attached) started throwing rebuild errors (I'm assuming cause the original construction geometry was altered).  Trying to repair the sketch, there were some little line segments within the construction line outline and some gaps.  So I fixed those.  But I'm still getting errors, and if I try to edit the offset value in the sketch it tells me "Reversing this offset would result in invalid geometry.  The previous sketch state has been restored."  I get this error for any attempted change whether reversing direction or not.

       

      Any help to solve the immediate problem?

       

      Is there a way in the future that if I use some reference geometry to build a part, that I can then break the link such that changes to the reference geometry won't enact further changes on the other part?

       

      Thanks!

       

      [Edit: I've repaired it myself through a brute force method, which wasn't elegant or pretty, but works.  However, if someone can answer the bolded question, I'd really appreciate it]

        • Re: Help repairing sketch
          Christopher Culver

          I noticed that you used splines instead of simple fillets for the corners?

           

          Also you can break the links between sketches by using the display/delete/add relations commands.

            • Re: Help repairing sketch
              Tom Gagnon

              Agreed, the Display/Delete Relations tool is what is needed.

               

              In that tool, use the drop down to filter it down to External references. Delete all from there.

              Then, add dimensions to fully define sketch. I prefer to place dims from primary planes within that part, to redefine it without context.

              Sometimes I apply the given dimension to keep it in place, sometimes I perform Measure inquiries and apply those to redefine it to where it belongs.

            • Re: Help repairing sketch
              Vladimir Urazhdin

              One click way to break all references:

              RMB on part in Feature Manager Design Tree ->List External References:

              Untitled.jpg

              Break All:

              Untitled1.jpg

              Now you model is clean and free from external references but still has internal references only

              • Re: Help repairing sketch
                Tyler D.

                All great answers, thanks!

                 

                (As for splines vs fillet, it wasn't a conscious decision, from what I can tell: On the enclosure that I derived this PCB from, I applied a constant radius fillet to an edge on the drafted part.  Using the measure tool, I only get arc length/chord length, but no radius like I do if I did this to an undrafted part.  So I'm guessing SW changes it to a spline automatically.  If I do a sketch fillet then extrude with draft, I can still measure a radius, but now it's not constant through the thickness of the extrusion

                [EDIT: a bit of thinking and now this makes sense - constant radius on a drafted edge means it's a section of a cylinder with the axis tilted away from the normal to the face due to draft.  So the cross section of this cylinder projected on the face = ellipse not a circle).