7 Replies Latest reply on Dec 4, 2014 7:13 PM by Jordan Gibson

    Big assemblies, creating single drawing files for pdf export etc.

    Jordan Gibson

      Hey guys, I need to find an effective way of doing this as Im taking way to much time with getting my drawings looking good.

       

      Basically I build Docks/Marinas so I create all my parts and their drawings, then make a small assembly for a section, and then create a large assembly to make sure all my sub assemblies fit.

       

      all this to say. At the end I want to make nice binders to send to my fabricators. So I have all these drawing files with a auto BOM at the top Item 1: -> Short descrip -> Qty: 1. Is there a way I can have solidworks bring these drawing files into one drawing file? I "Create drawing from SW assembly", do the auto balloon, get a nice BOM parts list with the quantity's of everything and nice item numbers. Now I need to take my individual part files I have, bring them in, get the item numbers and qtys updated, export to pdf and move on. Whats the easiest way to accomplish this?

       

      Thanks everyone!
      Jordan.

        • Re: Big assemblies, creating single drawing files for pdf export etc.
          Glenn Schroeder

          You can copy sheets from the part drawings and paste them into the assembly drawing to create a multiple sheet drawing, and you can link these part drawing views to the assembly BOM so the balloons will match.  Does that answer your question?

          1 person found this helpful
            • Re: Big assemblies, creating single drawing files for pdf export etc.
              Jordan Gibson

              Thats definitley a start. So I can just Ctrl C and Ctrl V. Im not going to make and dependencies by accident and ruin anything? Also I guess I would need to manually adjust each BOM line item with the correct item# and Qty#?

                • Re: Big assemblies, creating single drawing files for pdf export etc.
                  Glenn Schroeder

                  Right-click on a sheet tab and select Copy from the drop-down.  Go to the assembly drawing and right-click on a sheet tab.  Choose Paste.  You'll get a dialog box asking where to Paste it.  Make the appropriate selection and the sheet will be pasted in the drawing.

                   

                  Not sure what you mean about dependencies.  Assuming that the part drawing and assembly drawings reference the same parts, and they should, you shouldn't have any problems.

                   

                  For the item numbers, after pasting the part drawing sheet, right-click on the part drawing view and choose Properties.  That will take you to a dialog box where you can link the drawing view to the assembly BOM so that the balloon on the part view will match the BOM.  You shouldn't need to manually adjust anything.

                    • Re: Big assemblies, creating single drawing files for pdf export etc.
                      Jordan Gibson

                      So the copy paste works ok, I get the views and measurements, however the my sheet titles are missing. Also if I right click and go to properties and select the BOM that is used for the assembly. Nothing changes. Even if I apply. refresh and make a new BOM of that view its all the same info.

                        • Re: Big assemblies, creating single drawing files for pdf export etc.
                          Paul Cullen

                          Hi Jordan

                           

                          Your BOM is referencing your main assembly creating or copying drawing sheets does not change your main assembly so you BOM does not change. Your BOM will only change if you add or remove parts from the assembly. By right clicking on a drawing view and selecting the BOM to reference this only makes sure that any balloons attached to that view are numbered correctly as per your BOM.

                           

                          The reason you are missing your sheet titles is probably because there are notes in your sheet format that have properties linked to them, such as file name etc. If these properties were created using the option "Current document" when choosing the property to link to, your drawing sheet will now link the properties to your assembly instead of to your part. You could try creating a new sheet format and make new notes with linked properties but use the "Model in view specified in sheet properties" to link the properties to. You can then use this new sheet format for any sheets that you want to have your notes linked to the individual parts instead of the assembly.

                           

                          properties.JPG

                           

                          If you already have your drawings created you could save them out as pdf files and then merge them into one pdf file http://www.wikihow.com/Merge-PDF-Files

                           

                          Paul

                  • Re: Big assemblies, creating single drawing files for pdf export etc.
                    Jeff Holliday

                    I suggest creating individual drawings for each part/subassy/assy and then combining the resulting individual pdf files into one documentation book. Most all pdf creation programs could do this.

                     

                    Combining multiple parts/assy's into one SW drawing can lead to large files and missing links. Also if one part changes it is only necessary to pdf that part's drawing and cut/paste it into the pdf doc book.