10 Replies Latest reply on May 17, 2007 6:01 PM by henk kemper

    convert model edges to sketch entities

    henk kemper
      Is there a way to convert edges of a assembly-model to a sketch?

      A "workaround" I use now is: I make a drawing of the assembly, save it as dxf, start autocad, open the dxf, copy with control+c the entities to the clipboard, open a new sketch, paste the entities to the sketch.
      But there must be a much easier way to do it???


        • convert model edges to sketch entities

          Start a sketch in an assembly, click on the edge you want then convert entities.

            • convert model edges to sketch entities
              henk kemper
              For a few lines it is possible, but the problem is I want convert the edges of a complex sub-assembly (with more than 1000 parts and sub assemblies). To select each edge of it is a lot of work!

              The reason why I want to use a sketch is to increase speed; when we engineer a new machine, we need other sub assemblies to determine where machineparts can be located. By using a sketch of those subassemblies instead of the complete model, Solidworks doesn't need to load all the parts of those sub assemblies.

                • convert model edges to sketch entities
                  Charles Culp
                  I don't understand your complete intent for creating the sketchlines, it sounds like you might want to try things like"lightweight" for all your subassemblies.  This willload the geometry, but not the features behind it.  If doneproperly, large assemblies will load in 15 seconds (orless) lightweighted.
              • convert model edges to sketch entities
                Open the assembly file, right-click and edit part, open a new sketch on the part face, convert entities on that one face (which can become your top/right/front view later). Open the part template file, paste the sketch. You can select all converted edges with window in the assembly file and perform CTRL C function. to copy entities. Then, in the part file, select the face you want the sketch to appear on, insert sketch, paste the entities using CTRL V. On your 2D to 3D toolbar in you part file, you can select the sketch and then select the "extrude" button. you can use the "align sketch" button to align the sketches so that the top and right side line up, for example. If you don't select the view before pasting the sketch entities, then you have to select the "front" view button on the 2D to 3D toolbar to add certain entities to the front plane.

                This sounds like alot, but is actually alot easier and faster than saving as dxf....as you mentioned earlier.

                Hope this helps!
                • convert model edges to sketch entities
                  Kelvin Lamport
                  You could also save the assembly as a part using the Exterior faces Only or Exterior components option. That way the full 3D effect is maintained, not just a 2D profile.

                  Or if you really prefer the 2D approach;
                  Select the drawing view
                  Use the Edit > Copy to DWGeditor function
                  Paste it into DWGeditor
                  Copy back to the SW model.

                  But I prefer Charles method of using the assy model in lightweight.
                    • convert model edges to sketch entities
                      Charles Culp
                      To expand on what Kelvin just posted.  If you *really* want toget the sketch information as lines... you can:

                      Open the assembly.
                      Save As... then select .sldprt.  save it with all thegeometry
                      Open up the newly saved .sldprt
                      Start a 3D Sketch.
                      Press F5, then select the second option, which is"Lines"
                      Now do a drag-select over the entire "part", which willselect every line.
                      Click on "convert entities".

                      You will now have a 3d sketch of every edge in the oldassembly.
                      -I haven't actually tried this, but I'm pretty sure it willwork.