11 Replies Latest reply on Aug 8, 2017 8:29 PM by Habib Ghalamkari

    Insert PEM nut into Assembly

    John La Grou

      New to SolidWorks. Just created a sheet metal part with lots of holes and bends and flanges, etc.. Very intuitive! A huge improvement from AutoCAD 1988, the last time I worked with CAD.

      Now I want to insert some PEM nuts (S) and PEM standoffs (SO) into some of the holes I created (sized for PEMs).

      I saved the part as an "assembly"

      When I open the assembly, I can no longer find INSERT / DXF option (PEM provides DXF files for their PEM nuts and standoffs).

      How do I insert PEM DXF parts into a Solid Works assembly?

      Tks,

        • Re: Insert PEM nut into Assembly
          Michael Lord

          John,

          Are you on SW Professional?

          Hole Wizard has PEM sized, so you can specify the size in that.

          PEM Holes.png

          Create a new Assembly/ Insert the part into a Assembly

          Toolbox then has PEM fittings.

          PEM TOOLBOX.png

          These drag & drop into the PEM sized hole in the Assembly and should auto size but can be configured

          PEM Fitting.png

          • Re: Insert PEM nut into Assembly
            Steve Calvert

            I wouldn't be using PEM DXF files in the first place, I use their .step files and make them SW parts so as to insert them into an assy made up of your sheet metal part and the nuts.

             

            Steve C

              • Re: Insert PEM nut into Assembly
                John La Grou

                Yes, everything worked perfect. The PEMs just snapped magically into place. But this is the first time I've created an assembly, so it brings up a work-flow question. Let's say I build a sheet-metal chassis (holes, folds, flanges, etc.). The chassis part is now done, but needs PEMs. I save the chassis "part" as an "assembly." Now I add all my PEMs to the assembly. Great. But let's say I now need to add a hole (or whatever) to the chassis. I see no "hole wizard" in the assembly screen. How do I make edits to the original chassis after its been made into an assembly (while retaining the added PEM nuts)?

                  • Re: Insert PEM nut into Assembly
                    Michael Lord

                    Instead of making one Assembly, make your chassis part with PEM fittings an assembly

                    Assembly-Sub Assembly.png

                    It then becomes a "sub-assembly" when inserted into the main assembly

                    Elec assembly.png

                    • Re: Insert PEM nut into Assembly
                      Bill Toft

                      To add more holes, just open up the sheet metal part and add them there.

                      My work flow is to create a separate sketch on the face of the part to define my hole locations (fully dimensioned) with one point for each hole. I name it "Hole Locator Master Sketch". Keep this sketch visible.

                      Start Hole Wizard and select that face. On he first tab, specify the hole details. Then, on the second tab (specify hole locations) I click on each point in my Hole Locator Master Sketch . This adds a point to the locations sketch for the Hole.

                      Later, to add more holes, first I update the Hole Locator Master sketch, then edit the hole locations sketch to add new points coincident with the new points in Hole Locator Sketch.

                      Advanced topic: In the assembly, add the first PEM & mate it. Make the hole locations sketch visible. Now use a Sketch Driven Pattern to locate all the other copies of that PEM.

                      Note that you can use a single Hole Locator Master Sketch to define all hole locations (no matter what size). Then, for each hole size, just click on the locations you want.

                      Later, if you need to move existing holes around, just edit the dimensions in Hole Locator Master Sketch. Magic!

                      • Re: Insert PEM nut into Assembly
                        Habib Ghalamkari

                        You can always click the chassis and select Open Part to open the part in a new window and edit it as usual or select Edit Part to edit it within the assembly.

                        2017-08-08_9-03-51.jpg

                          • Re: Insert PEM nut into Assembly
                            John La Grou

                            Habib, Bill, Michael: three different approaches and all excellent. Thanks so much. Now I have to figure out why yesterday's Base Flange build referenced dimensions from sheet metal OD, but today's Base Flange build is referencing dimensions from sheet metal ID (requiring a manual dimension adjustment for metal thickness). Must be a check box somewhere.

                             

                            Also looking for place to set system defaults (3-place tolerances, etc.). Right now, the default for all new drawings is set to two-decimal-place tolerance, and I have to manually change it for each drawing using the IPS tab.

                              • Re: Insert PEM nut into Assembly
                                Habib Ghalamkari

                                John La Grou wrote:

                                 

                                Also looking for place to set system defaults (3-place tolerances, etc.). Right now, the default for all new drawings is set to two-decimal-place tolerance, and I have to manually change it for each drawing using the IPS tab.

                                You need to correct your drawing template or add a new template.

                                Create a new drawing using an existing template, click the gear button and then options.

                                In options, click Document Properties and then select Dimensions.

                                You can change the primary precision three.

                                When you are finished, over write the current template or save it as a new template.

                                 

                                Now when you need a drawing, use this new template and you're OK.

                                 

                                2017-08-09_8-21-54.jpg

                                  • Re: Insert PEM nut into Assembly
                                    John La Grou

                                    Habib, thanks. Got it. Seems unintuitive that a unique template is required to achieve one's standard dimensionals. Ideally, simply opening New / Part should bring up one's saved default working space. No?

                                      • Re: Insert PEM nut into Assembly
                                        Habib Ghalamkari

                                        John,

                                        You may use just one type of drawing/part file but users may need different settings for different cases.

                                        For example our drawings which are going to be sent to Asian companies are in metric, otherwise we use Inch.

                                        The position of BOM, Revision tables, etc are different too. we have different structure of drawings for  sheet metal too, because we need to send the flat pattern and hole table to the shop floor.

                                        So we have different templates which we use at different situations. It allows us to have control on what we are trying to do.

                                         

                                        Without templates, we were in trouble.

                                        So one more click to select a template is much more better than having a system wide settings which is used in all drawings.