16 Replies Latest reply on Oct 26, 2018 11:55 AM by Wayne Bird

    Part drawing with multiple configurations

    Wayne Bird

      I have a part that has multiple configurations (not in a design table).  The configurations are a simple change in some dimensions.  How do I create a table that will show these variable dimensions, i.e., A, B, C?

        • Re: Part drawing with multiple configurations
          Jeremy Feist



          1. Add a design table to the part, and show that (there are some tricks to getting it formatted correctly.
          2. add a SW table and start typing.
          3. make an excel table and insert it into the drawing.
          4. make an excel table and copy paste the values into a SW table on the drawing.
          5. ???


          only option 1 is linked to the dims in your configurations.

          • Re: Part drawing with multiple configurations
            Rubén Rodolfo Balderrama

            maybe I was wrong...like this?

            • Re: Part drawing with multiple configurations
              Jim Sculley

              For what it worth, when I create a tabulated drawing (which I don't do often) I eliminate the configurations and do it with an assembly and a custom BOM.  The model often starts as a configured part but they are saved out as separate files to maintain our one file per part number rule and to allow it to work properly with some automation associated with EPDM.  An assembly is created that includes all of the models and a drawing of that assembly is created as the tabulated drawing.  The overall process looks like this:


              1. Create a part model for one of the parts to be listed on the tabulated drawing.
              2. Click on File...Properties to open the Custom Properties dialog.
              3. Click on <Type a new property> and enter the text 'A', including the single quotes.
              4. Click in the Value/Text Expression column.
              5. In the feature tree, click the feature that has the dimension that needs to be tabulated. If necessary, move the Custom Properties dialog to one side, or to your second monitor so that you can see the feature tree and the model.
              6. In the SOLIDWORKS graphics area, select the dimension to be tabulated. The dimension name (e.g. "D1@Boss-Extrude1@Part1.SLDPRT") should appear in the Custom Properties dialog.
              7. Repeat steps 3 through 7 for any other tabulated dimensions, using other property names such as 'B' and 'C'.
              8. Click OK in the Custom Properties dialog.
              9. Perform a Save As or Save As Copy of the model for each item that will appear in your tabulated drawing.
              10. In each model, change the tabulated dimensions as necessary.
              11. Create a new assembly model and insert each of the tabulated item models into the assembly.
              12. Hide all but one of the models in the assembly.
              13. Save the assembly.
              14. Create a new drawing from the assembly.
              15. Dimension the drawing as normal, but for the tabulated dimensions override the dimension text with the custom property name defined in step 3 above.


              The next few steps rely on a custom BOM  template we made for tabualted drawings.  It simply has a columns linked to the custom properties defined in steps 3 through 7 above.


              16. Select a drawing view and Click Insert...Table...Bill of Materials.

              17. Click the Star button in the Table Template area of the property manager.

              18. Select the TABULATED DRAWING template.

              19. Click OK and place the table on the drawing. It should already be populated with your tabulated item information. The table will respect the units defined in your model. For example, if you want to have fractional inches for one of your tabulated dimensions, simply override the dimension display in the model to use fractional inches.

              20. The default template includes only one tabulated dimension column. If you need more, insert a new column in the table, make sure Column Type is set to Custom Property and select your custom property (e.g. 'B') from the drop down list.

              21. Save your drawing.

                • Re: Part drawing with multiple configurations
                  Wayne Bird

                  Thanks Jim for the input.  We have a ton of tabulated autocad drawings that we're converting to SW.  The SW configuration feature seems to be well suited for this very purpose and saves on a ton of individual files. It seems like your method defeats this purpose, but maybe I'm missing something here?

                    • Re: Part drawing with multiple configurations
                      Jeremy Feist

                      it comes down to a couple of points

                      1. are you using a PDM system? does that PDM system allow different configurations to have different revs (SW PDM does not out of the box)?
                      2. do you currently have different revs for the different part numbers in one table, and/or want that option in the future?

                      Jim Sculley specifically said that have a rule of one file per part number. so that is their method. we also have tabulated part drawings and use SW PDM pro, but do not have that rule, so we use configurations. (our rule is 1 drawing per part/assembly).