12 Replies Latest reply on Feb 26, 2014 8:31 AM by Rick Becker

    Change all views in SolidWorks drawing to 1:1 scale, export as dwg

    Thomas Malinski

      I have been looking over the many macros and discussions on saving SolidWorks drawings as AutoCad dwg files at 1:1 scale. But I have not found any that will do what I'm looking for with mixed scales on one sheet

      I need a macro that will save a slddrw sheet as a dwg for AutoCad but will change all of the various model view scales and or sheet scale to be 1:1.

      In our company we plot multiple detail components on a single D size sheet. We cram as many details as we can fit on a single sheet and we adjust each model view scale depending on how large or small the component is. It is not uncommon for a D size sheet to contain 15 deatils with 4 or 5 different scales as necessary for clarity for the toolmaker. There may also be an overall sheet scale that is not 1:1 this should also be considered for an unconditional conversion to 1:1 for everything in the sheet

       

      Once in Autocad I typically delete the frame and all annotations and dimensios and hatching so all that is left is 1:1 geometry for CNC toolpaths

      I supply our CNC department with a paper print of the SolidWorks drawing with annotations and machining instructions, but the cleaned geometry is from my converted AutoCad dwg file.

       

      Any help is greatly appreciated

      Tom Malinski

        • Re: Change all views in SolidWorks drawing to 1:1 scale, export as dwg
          Anna Wood

          What software does your CNC guys use for tool paths?  They can't use the solid model in their software?

           

          Seems like a ton of extra work when most CAM software these days can read in a solid model for cutter path generation.

           

          I know I am not answering your question.  Just surprised you are still sending you CNC guys 2D cad in this day and age.  :-)

           

          Cheers,

           

          Anna

            • Re: Change all views in SolidWorks drawing to 1:1 scale, export as dwg
              Thomas Malinski

              Hi Anna, we use Mastercam and it works very well for Solid Models in our CNC Milling dept, However, in our WEDM dept they have a hard time with Mastercam and models. We are in the process of considering making a change to DP Esprit just for WEDM, but change is slow. So in the mean time I've been tasked to try to automate the conversion to dwg for WEDM.

              Regards

              Tom Malinski

                • Re: Change all views in SolidWorks drawing to 1:1 scale, export as dwg
                  Christopher Estelow

                  Thomas,

                     I have to do the same thing at my job for Wire EDM but I don't have to do any annotations or notes.  What I typically do is just a blank drawing with all of the views I need in 1:1 scale.  That way my machinist can delete what he doesn't need. 

                   

                  Chris

                    • Re: Change all views in SolidWorks drawing to 1:1 scale, export as dwg
                      Thomas Malinski

                      This would be good for me also, The big nut is to make sure multiple model view scales are all converted to the same 1:1 scale in the DWG file

                      Regards

                      Tom

                        • Re: Change all views in SolidWorks drawing to 1:1 scale, export as dwg
                          Anna Wood

                          We use Esprit for our wire work.  We haven't sent a dxf/dwg to wire in close to ten years.  This would be a great choice for you guys.

                           

                          The trick to making this work is to model your wire starts and have two configurations in your sldprt files.  One for Milling and then the final default configuration.  Esprit can bring both configurations into the same file to set up wire paths.

                           

                          Modeling your wire starts and milling configuration has the added benefit of keeping the designer aware of how the parts are going to be milled and wired. Keeping unmanufacturable designs being sent to the shop down to a minimum.

                           

                          Here is an example sldprt and slddrw.  For the plan view there are two views overlaid.  The Milling Operation configuration is used to generate the hole chart.

                           

                          Cheers,

                           

                          Anna

                            • Re: Change all views in SolidWorks drawing to 1:1 scale, export as dwg
                              Thomas Malinski

                              Anna, funny thing our models and drawings for CNC are very similar to what you linked. We use a WEDM configuration and a Mill Config along with the Default config if the detail requires it. We create our drawings very similar to yours. The only huge difference is we convert our drawings to Autocad for WEDM programming of Toolpaths. Milling can work with our models directly with Mastercam. However we still have many designers using autocad, that's another story! So our mill department gets a mix of models and 2d

                              Thanks for taking the time to share your methodologies with me. I appreciate it.

                               

                              Tom Malinski

                              • Re: Change all views in SolidWorks drawing to 1:1 scale, export as dwg
                                Rick Becker

                                Anna,

                                 

                                Thank you for posting your solution.

                                 

                                We are new to SolidWorks having used it for only about a year. Coming from freeform modeling and 2D design it has been quite a learning curve.

                                 

                                In order to get geometry to our Wire EDM's, we have been saving our drawings out of SolidWorks as DXF, opening then in KeyCreator, deleting everything except for the needed geometry, fixing line thickness problems, changing color and exporting as DXF. (we have a macro (in KeyCreator) that does most of this and more)

                                 

                                There must be a better way.

                                 

                                When I opened you drawing (218930, Die Insert, Gut and Lance.slddrw) I noticed that you have  2 drawing views (Drawing View 1 & Drawing View 5) on top of one another, each from a different configuration.

                                 

                                I discovered that you can right mouse click on one of the instances, select Alignment and click on Align Horizontal by Origin (or Center). Hold CTRL and select the other drawing view.

                                 

                                Repeat that and click on Align Vertically by Origin (or Center).

                                 

                                Both drawing views are aligned, but only in one direction.

                                 

                                I could then right mouse click and select Lock View Position on both drawing views.

                                 

                                Is this how you position the drawing views? I can only lock the position in either Vertical or Horizontal, not both. Am I missing something?

                                 

                                How are you assured the views are aligned Precisely? Any misalignment going to manufacturing will be expensive.

                                Have you ever had the views not aligned?

                                 

                                Does Esprit allow you to choose the configuration to load when opening SolidWorks files similar to how MasterCam asks?

                                 

                                I know you don't export any DXF files, but if we exported DXF files from a drawing with multiple drawing views on top of one another, would we have line over line for common edges and holes? How would MasterCam Wire (or Esprit) handle that? (I noticed that the exterior lines of Drawing View 1 are not visible but the round holes are).

                                 

                                Thank you in advance for any insight you can offer  It is greatly appreciated.

                                  • Re: Change all views in SolidWorks drawing to 1:1 scale, export as dwg
                                    Anna Wood

                                    Rick,

                                     

                                    We align to origin both vertical and horizontal.  You have to be a bit careful when motoring around a drawing not to move the views out of alignment.  Not a huge deal, it happens every once in a while.  You have to re-align the views.  I am so used to working this way (for many years) that I do not think to much about it.  I might move a view out of whack a handful of times over a year. 

                                     

                                    If that is a concern about the views getting out of alignment, create a two sheet drawing.  One sheet shows the Milling Op views and the other sheet shows the Final finished views.

                                     

                                    I know our CNC and wire people really like the two configurations.  Makes it very easy for both groups to understand what needs done and what they are getting from each other.

                                     

                                    You can import a solid model multiple times into Esprit.  Esprit will give you a choice on which configuration to load.

                                     

                                    I do not have an issue with multiple lines because I would not send DXF files.  For your situation I would do a two sheet drawing and not overlay the views.

                                     

                                    Cheers,

                                     

                                    Anna

                                • Re: Change all views in SolidWorks drawing to 1:1 scale, export as dwg
                                  Anna Wood

                                  Not sure why the mutiple view scales would be an issue if you are setting up a dedicated wire only sldddrw that has nothing to do with your dimensioned and detailed slddrw.

                                   

                                  All views generated for this wire only slddrw would be placed at 1:1.

                                   

                                  It is basically pick your poison.  Set up two different slddrw's for your audience or spend time making sure all your exported dxf's are at 1:1 scale.

                                   

                                  I would be campaigning real hard to get Esprit into your wire room.  Takes all the extra data translation work away. 

                                   

                                  Cheers,

                                   

                                  Anna