6 Replies Latest reply on May 16, 2017 5:57 PM by Jason B.

    Error in small dimension for offset entities

    Dustin Dobransky



      I am designing a box to be laser cut with 1/4" acrylic.  I use a box joint, which requires a very precise offset from the original dimensions of the box to account for laser kerf (width of the laser beam).  I am using SW 2015.


      To accommodate for laser kerf I follow these steps:

      1. create a new subconfiguration of the original-dimensioned part

      2. click a face of the part>sketch>convert entities to get an outline of the part.

      3. offset entities, set thickness to global variable "laser_kerf_quarter_inch_acrylic", which is 0.0025"


      After I click the little green arrow, I get the message: "identical contours in the same sketch are not allowed for this operation".  It seems like unpredictable behavior, as this happens with some parts and not others.  Sometimes I can restart solidworks, restart steps 1-3, and I won't get the error.  Sometimes I set the offset to 0.005", exit the sketch, rebuild, re-edit the sketch and change the dimention to 0.0025", and SW will crash.


      Through trial and error, I found the minimum distance that this error will not happen at is 0.005".  I ran a test with this offset distance, and there is too much wiggle room in the acrylic to make for a strong bond using acrylic cement (which needs the material to be touching, i.e. no wiggle room).


      Any ideas on a permanent solution to this?


      Here are some pictures describing what I am talking about:


        • Re: Error in small dimension for offset entities
          Dustin Dobransky

          I found a workaround:


          1. Follow steps 1-3 from above, but set the offset to an equation: '=0.005"'

          2. Right click equations>manage equations

          3. Edit the new equation just created, set to "laser_kerf_quarter_inch_acrylic" (=0.00255")

          4. Rebuild

          5. Success.

          • Re: Error in small dimension for offset entities
            Dennis Bacon

            Dustin,, By the looks of your sketch you converted entities (around the periphery of the part) then offset that. This will work if you change the converted lines to construction geometry then offset, but I suggest starting a sketch on the surface, select an edge, select loop, then offset that selection of edges. Do not convert the edges. .0025 is fairly large number for an offset. I did it with .0005 and could have gone smaller than that. I'm not sure why you need the laser path (center beam) unless you are writing out your program and do not have offset capabilities on your machine conditions. I suppose there are some machines like this but I have never seen one.

            Edit:.. Are you getting interpolation errors without the center path? Seems unlikely since the intersections are perpendicular and obtuse.

            • Re: Error in small dimension for offset entities
              Derrick Formsoa

              Tom, I have been wondering the same thing. I was able in the past to create an equation to control an offset amount and apply it to many offsets in a single sketch.... I hope this gets resolved.

              • Re: Error in small dimension for offset entities
                Jason B.

                I have a similar issue, but it is currently when using convert entities in an assembly.  I'm using Solidworks 2016 SP5.


                I have an extruded part which is included twice in an assembly, and mated coincident to a planar surface.  Sketching on the planer surface, I can convert the end of one of the extrusions, but when attempting to convert the second, it gives me the error.  I tried converting entities on one, then using offset entities with a 0 offset on the other, to no avail.  I don't see any reason why this is an issue.  So far, 2016 has proven to be an all around headache.  So tired of changing the way we approach designs to suit undocumented or unexplained changes in Solidworks between versions.  I understand the errors are generic because of the way Solidworks is structured, but...   that is another conversation.  I digress...