11 Replies Latest reply on Feb 23, 2017 3:27 PM by Mike Pogue

    Drafting Standards file doesn't update "Units"?

    Eddie Pellegrin

      I was under the impression that everything under the "Document Properties" tab could be saved as a "Drafting Standards" file and loaded into each drawing. How come if I change my dual dimension units from millimeters to inches (when my standard is set to millimeters) and then re-load my drafting standard, it doesn't update dual dimensions to millimeters. It keeps them at inches? Solidworks 2016 SP 5 here.

        • Re: Drafting Standards file doesn't update "Units"?
          Dan Pihlaja

          I believe that this portion is saved in your part/drawing template and NOT your drafting standard.




          Snippet from the link:

            • Re: Drafting Standards file doesn't update "Units"?
              Eddie Pellegrin

              After reloading the standard didn't work, I thought about the template also. However, if I load a new drawing template, then change the dual dimension units to inches, then reload the template, the units also stay inches.

                • Re: Drafting Standards file doesn't update "Units"?
                  Cad Admin



                  Are you "starting a new drawing" or opening the .drwdot template file? After you changed the units, did you resave the template file?


                  Dan is correct in the delineation of Dimension standard to template settings

                    • Re: Drafting Standards file doesn't update "Units"?
                      Eddie Pellegrin

                      I am starting a new drawing which pulls up our .slddrt (title block) files. Is there a way to start a drawing using the .drwdot? and how would you reload the .drwdot on an existing drawing, is that possible? Thanks for helping by the way.

                        • Re: Drafting Standards file doesn't update "Units"?
                          Cad Admin

                          We always use the .drwdot files.  We just put all of them in a central folder and under "system properties" in "File Locations" Set the "Document Templates" to the folder where your templates are.


                          They should then appear in your New file dialog box.

                          (sorry i would add screen shots but my capture tool is erroring out)

                          • Re: Drafting Standards file doesn't update "Units"?
                            Glenn Schroeder

                            If you're starting new Drawings then there's no reason to reload a drafting standard.  The new Drawing should open with all the same settings at Tools > Options > Document Properties that were active when the Drawing Template was last saved.


                            And yes, new Drawings should be started with the saved template (.drwdot).  That's what they're for.  When you start a new document, if you're seeing this:



                            Then click on the "Advanced" button in the lower left corner.  That will take you to a dialog box where you can choose from your saved document templates.  If they don't show up there, then you aren't pointing to the correct location at Tools > Options > File Locations > Document Templates.


                              • Re: Drafting Standards file doesn't update "Units"?
                                Cad Admin


                                Thanks for the added screenshots...lol


                                Eddie, take a look at this post.

                                slddrt visit drwdot

                                  • Re: Drafting Standards file doesn't update "Units"?
                                    Eddie Pellegrin

                                    I really appreciate the help guys, that makes sense. You see, this is what we are running into. We sometimes get drawings from other divisions in the company that don't use our drawing template or format files. So in the process of updating them to our standards, will load up our standards file and sheet format. In doing this, the standards file changes the dimensions to be dual dimensions. However, now I've learned that although the dual dimension setting is in the standards file under the "Dimensions" as seen in the above screenshot, the setting for the "type" of unit is found in the section that is controlled by the drawing template. So when we are running through updating one of these drawings, if someone from a different division set their dual dimensioning units to "inches", neither updating the sheet format or drafting standard file will update the dual dimension units. We were hoping that we could "load" up one or the other and have it fix this back to our standard, but from what I see, it appears that the only way to fix this is to manually go in and change it back to millimeters?

                                      • Re: Drafting Standards file doesn't update "Units"?
                                        Dan Pihlaja

                                        I am sure that a macro could be written to do this for you.


                                        I just did a quick record macro and changed the unit system to MMGS and then changed the dual units to inches.


                                        Dim swApp As Object

                                        Dim Part As Object
                                        Dim boolstatus As Boolean
                                        Dim longstatus As Long, longwarnings As Long

                                        Sub main()

                                        Set swApp = _

                                        Set Part = swApp.ActiveDoc
                                        Dim myModelView As Object
                                        Set myModelView = Part.ActiveView
                                        myModelView.FrameState = swWindowState_e.swWindowMaximized
                                        boolstatus = Part.Extension.SetUserPreferenceInteger(swUserPreferenceIntegerValue_e.swUnitSystem, 0, swUnitSystem_e.swUnitSystem_MMGS)
                                        boolstatus = Part.Extension.SetUserPreferenceInteger(swUserPreferenceIntegerValue_e.swUnitsDualLinear, 0, swLengthUnit_e.swINCHES)
                                        End Sub


                                        I am sure that you could do something similar.


                                        Then link the macro to a button on your toolbar (Or better yet, your "S" shortcut toolbar), and you are off and running.

                          • Re: Drafting Standards file doesn't update "Units"?
                            Mike Pogue

                            I actually know this one. When you save a drafting standard over an old one, it will not overwrite it. You have to delete the old one, then save the new one. For good measure, you might try changing the name--I haven't changed my drafting standard in years.


                            This is a very old bug, and I doubt it's going anywhere.


                            It is not possible to reload a template on an existing drawing, and there is no distinction between the settings saved in the template or part file and this saved in the drafting standard. The drafting standard file is basically a macro to go through and set the settings in the part file or template.