8 Replies Latest reply on Feb 14, 2017 6:26 AM by Zac Aj

    Negative Space/Holes from part w/o Smart Feature

    Zac Aj

      A bit new to solidworks, hopefully this makes sense...

       

      I'm working on a project where I'm going to have 200+ parts mounted on a sheet of plywood, and wanted to use a CNC router to pre-drill all the screw holes and cut out regular holes of various shapes for the parts for easier assembly.  Although there's a lot of parts, there aren't that many different ones, and most would probably have 5+ separate cuts/screws necessary.  What I was hoping to do was to model each part, including some 'negative space', so that when I added and positioned the part on the board in the assembly, it would automatically leave those cuts in the wood, but I don't see any obvious way to do this.  After a lot of searching I came across Smart Features, which seem to be trying to solve vaguely the problem I have, but they're very cumbersome.  It seems that, for every one of the parts, I'd have to repeatedly insert them into the assembly, mate and position them, then select 'Insert Smart Feature', and then select the same set of faces on my board so it knows how to insert the holes from that part, even though this information isn't changing at all from part to part, and it generally seems overpowered for the simple needs I have.

        • Re: Negative Space/Holes from part w/o Smart Feature
          Glenn Schroeder

          I'm not real sure what you mean by "negative space".  If you mean that the parts that attach to the plywood would have bodies that protrude into the plywood and you want to use these to cut the plywood, that should work.  Edit the plywood part inside the Assembly and use the "Indent" feature to make the cuts, using the other Parts for the cutting bodies.  In the screenshot below I'm using the bolt to cut the concrete barrier.  Don't forget to select "Cut" in the feature's Property Manager.

           

          • Re: Negative Space/Holes from part w/o Smart Feature
            Steven Mills

            That is one way to do it. But there are a couple of other ways.

             

            This is the one I would do in your case;

            1. Position all the parts as you want them on the sheet.

            2. Then edit the sheet within the assembly, and start a new sketch

            3. Then use the 'Convert Entities' tool to make the holes you need using the edges and/or sketches of the parts your mounting.

            -This will give you one big sketch that gets input from all the parts you are using. May want to make a few sketches as you may be removing the parts in re-designs, and it's easier to just delete unused sketches than deleting 5 or moe lines in a sketch.

             

            The other method is a one to three step process. Though it will have to be repeated every time you make a change to this assembly.

            1. Position all the parts as you want them on the sheet.

            2. Save the entire assembly as a part. This will make a 'dumb body' part with many bodies in it.

            3. Use the 'Combine' tool in the new part to subtract the solid bodies of all the mounted parts from the plywood sheet.

              • Re: Negative Space/Holes from part w/o Smart Feature
                Zac Aj

                With the first method, it seems to me (as with Glenn's suggestion above), that I would need to manually go through and select every intersecting entity every time I added a part, to make the sketch, is that correct?

                 

                The second method seems like it could be workable, in theory.  It's not like I'll be making these boards very often, so a few extra steps to 'export' the cut board aren't that bad (as long as they don't require extra work for each part, like the other methods seem to), however I'm not having any success trying it.  I made a simple assembly with a sheet of wood and one part intersecting it, and then did File->Save As and chose Part from the file type dropdown.  Then I opened the newly saved part, which contained a long list of surfaces instead of some bodies, which surprised me, and when I went to use the Combine tool it was disabled.  I googled about it being disabled (wish Solidworks would tell me instead of just graying them out...), and the problem seemed to be that I only had one part?  Which if course I did, since I'd just made my assembly into one part.  Did I go wrong somewhere along this path?

                  • Re: Negative Space/Holes from part w/o Smart Feature
                    Steven Mills

                    To the first method. Yes, but it's really easy to do. Though it might take almost an hour with 300 parts. *shrug*

                     

                    To the second, huh. I'm guessing you had 'Exterior faces' option checked when you saved from the SLDASM to a SLDPRT file?

                     

                    I am able to do those steps using SW 2016 and when I don't have any options selected like the above picture, I get a feature tree like this;

                    Notice the solid bodies? And that there are no surface bodies? If you don't have solid bodies in your model/part, tools that need solid bodies like the 'Combine' tool will be grayed out.

                      • Re: Negative Space/Holes from part w/o Smart Feature
                        Zac Aj

                        Ah, that does it, thanks!  When I saved it I didn't have anything selected in the options there either, but on mine (2015) apparently that makes it export the faces.  Selecting 'All components' produced a similar part with all the solid bodies, and then I was able to do a Combine and subtract everything else from the sheet by just using CTRL+A.  As long as I make sure to make special extra bodies in my parts for the 'subtraction' I think this should work.