9 Replies Latest reply on Mar 31, 2015 1:21 PM by Cliff Behrend

    Referencing in solidworks using excel

    Raghav S


      I would like Solidworks to generate a profile as attached below using dimensions that i input on excel.

      For example i would enter the following for the below profile

      Depth: 6.8mm

      Radius: 6.75mm

      Bottom Radius: 10mm

      Fillet Radius: 0.8mm

      Angle between the upper line and the vertical: 85'

      On entering the above parameters on excel, is it possible that solidworks will generate the profile as shown?

      My aim is to change these parameters and obtain a corresponding profile so that i don't have to repeatedly draw the profiles.

      If yes, How do i go about it?



        • Re: Referencing in solidworks using excel
          Wojciech Nieroda

          Hello Raghav,

               You can do it via Excel.

          1. First you must insert the Design table (menu Insert - Tables - Design Table)

          2. You can change options in the Design table property manager. I'm using Auto-create option.

          3. After applying Design table, SolidWorks will show you Dimensions window. In this window select dimensions that you want to change through Excel.

          4. After adding them to the design table, you can change them. Closing Design table will force update your sketch.

          5. If you skipp some dimensions, you can open Design table (Configuration manager), set cell to the first empty cell in the second row, show dimensions through SolidWorks tree and click dimension that you want to add to table (click once if the Instant 3D button is active and twice if not). If you open Design table in its own window, you must add items to table by clicking twice.

          6. This table is saved internally in part/assembly


          Hope that it is what you wanted.

          Kind Regards,



            • Re: Referencing in solidworks using excel
              Raghav S

              Thanks Wojciech Nieroda. Also there is another problem. Based on changes to the above profile, the design of another part with which it mates must also change and the changes have to appear in the assembly. How do i link the two? Also it would be easier if i could specify all inputs at just one location, say the assembly file and the changes in the part part files occur automatically using those inputs. Is it possible to do so?


                • Re: Referencing in solidworks using excel
                  Wojciech Nieroda


                  Yes it is possible. You can try to do it via global variables only, you can drive one part through global variables, and other parts link to first part in context of the assembly, you can create notepad file on your drive and put parameters to this file and then link this file to all parts/assemblies that need to use some or all of parameters.

                  The easiest way is first.

                  In the assembly level go to the equations dialog and then create all global variables that you need.

                  Then in the assembly level show feature dimensions that you need to link to global variables (double click on operation or face of the feature)

                  Modify dimension, type = sign and select or type global variable name. Do the same for all other dimensions.

                  Then, if you want to change some of these dimensions, you must do it from assembly level (equations dialog for example)


                  Kind regards,


                • Re: Referencing in solidworks using excel
                  Marco Gigante

                  what's Wojciech Nieroda say is correct but please keep in mind:


                  - if you just change manually parameters on excell sheet, it will work perfectly

                  - if you obtain this parameter from an excell formula, it's possible that won't work due to the fragile compatibility between solidworks and excell

                    • Re: Referencing in solidworks using excel
                      Cliff Behrend


                      Create your model as needed



                      Design 1.JPG



                      Create new excel workbook (Single worksheet only)

                      Create Variable names in first column




                      Create variable values in second column




                      Save as a Unicode text file "Your Model".txt (Choose your own file name)





                      Open model

                      Manage Equations

                      Import "Your Model".txt

                      Save Equation box

                      Open drawing to be modified

                      Select dimension you want linked to variable

                      Repeat as needed for your model


                      Design 2.JPG



                      Save model


                      Hope this helps


                  • Re: Referencing in solidworks using excel
                    Kelvin Lamport

                    Use Top Down or In-Context modelling technique;

                    Create a sketch in the assy, controlled by a DT, with both parts referencing the sketch.