22 Replies Latest reply on Nov 19, 2018 12:56 PM by Shawn Stugard

    Configurations

    Chris Scougall

      I am just starting to explore the world of configurations, but I am confused about a few things. I created a model, then added a new configuration and modified it. I would think that the original configuration would be unchanged but the changes I made to the new one are reflection in the original. Did I do something wrong or leave something out?not sure where I went off the tracks.

        • Re: Configurations
          Dennis Dohogne

          Chris Scougall wrote:

           

          I am just starting to explore the world of configurations, but I am confused about a few things. I created a model, then added a new configuration and modified it. I would think that the original configuration would be unchanged but the changes I made to the new one are reflection in the original. Did I do something wrong or leave something out?not sure where I went off the tracks.

          When you change a dimension you have the option to change it for all configurations, just the current one, or to specify which configurations are affected.

           

          Do yourself a huge favor and go through ALL the built-in SWX tutorials, but especially the one on configurations.  It will answer probably 99% of the questions you will have.

          • Re: Configurations
            Steven McCallion

            Hi Chris,

            The simplest way to decide what configs are affected when you make a change, is enacted while you make the change.

            By default changes will affect all configurations.

            If you're changing a dim in a sketch for example, there's an option to the side of the measurement popup where you choose which configs the change will affect.

            There's many other ways to control the measurements of different configs, and for those I'll point you to the help files.

            /Steve

            • Re: Configurations
              Thomas Voetmann

              When you change dimensions you can select how other configurations will be influenced.

              Also you can suppress/unsuppress in different configurations and decide how new features will be handled.

              You have a lot of other options to control the difference between configurations, so welcome to an exiting and effective - but sometimes dangerous - new world.

              • Re: Configurations
                Ignacio Vital

                Hi Chris,

                 

                When you are working with configurations you have to take care of what implies each modification, it means you can do a change in a dimension for only a configuration, for especified configurations or for all configurations.

                 

                If you see the image below you will see there is a list where it appears for what configurations the number of the dimension is valid.

                 

                By default it is in all configurations, and that's why it happened what you describe.

                 

                 

                There are more information in Solidworks help, and in VAR blogs.

                 

                This link: 2018 SOLIDWORKS Help - Configurations can help you understand some things.

                 

                Regards,

                  • Re: Configurations
                    Chris Scougall

                    Thanks for the info guys, this is all great stuff. the way we were doing things here when we were using solid edge is to recreate a "finished Part" model from a customers blueprint and then save as individual separate models for all the individual machining operations (cut-off bar stock, lathe to finished diameter, mill face holes, mill OD holes, mill ID holes, etc.) . I thought that it would be best to create one part file with all of the different operations as a new configuration. I think I can use all of this helpful info. You guys are the best.

                     

                    Thanks again.

                  • Re: Configurations
                    Glenn Schroeder

                    Chris Scougall wrote:

                     

                    I am just starting to explore the world of configurations, but I am confused about a few things. I created a model, then added a new configuration and modified it. I would think that the original configuration would be unchanged but the changes I made to the new one are reflection in the original. Did I do something wrong or leave something out?not sure where I went off the tracks.

                     

                    It sounds like you didn't go to the configuration properties and select "Suppress features" (see near the bottom of the screenshot Thomas Voetmann posted).  I just read through your reply again.  If you're adding features to the new configuration, then that is still what you need to do.

                     

                    If you were referring to editing dimensions in existing features, then, as Dennis Dohogne and Steven McCallion said, changes to dimensions will affect all configurations unless you tell the software different.  My preferred method is to show the dimension in the graphics area (there are a couple of ways) without the feature being active.  Right-click on the dimension and choose "Configure dimension" from the drop-down.  That will open a simple table, with a column for the dimension and a row for each configuration.  You can set the desired value for each configuration in this table.

                     

                      • Re: Configurations
                        Chris Scougall

                        in the attached image, the red construction lines represent geometry from the original "finished model". basically what I am doing is offsetting certain lines to add material for a machining operation. in the end the operation will get modified down to the original part. is this the best way to do this? i can set new dimensions for that particular configuration, but the chunk of material in the lower right outside of the red construction lines are the same dimensions as the finished part so that feature is being carried back to the original. this part doesn't have any holes, but most of my other part do, which i suppress until that machining operation calls for them.

                         

                          • Re: Configurations
                            Shawn Stugard

                            The best way (IMHO) to do this method would be to start with an "as cast" or "as welded" configuration. Then you can add the various machining operations on the subsequent configurations to get down to your final size. Then you'll have a config for each step of production.

                            • Re: Configurations
                              Glenn Schroeder

                              Chris Scougall wrote:

                               

                              in the attached image, the red construction lines represent geometry from the original "finished model". basically what I am doing is offsetting certain lines to add material for a machining operation. in the end the operation will get modified down to the original part. is this the best way to do this? i can set new dimensions for that particular configuration, but the chunk of material in the lower right outside of the red construction lines are the same dimensions as the finished part so that feature is being carried back to the original. this part doesn't have any holes, but most of my other part do, which i suppress until that machining operation calls for them.

                               

                              As Shawn Stugard suggested, I'd have separate features to remove the material and/or add holes for each fabrication step.  Be sure you go into the configuration properties for each configuration and choose the option to suppress new features (see above).

                              • Re: Configurations
                                Ignacio Vital

                                Hi Chris,

                                 

                                My way of doing this thing is:

                                 

                                I always extrude the part with the measures which the part will go to the CNC machine. Then I generate operations I need to achieve the finished state of the part. I try to generate features for each possible variation of the part.

                                 

                                An example: In my part I have 2 holes through all I can do it with 1 feature or 2 features. If there can be the possibility that the part may not need sometimes one of the holes, for me, it should be in 2 features, so I can suppress in the configuration the hole I don't want to use.

                                 

                                With the configurations take care with the options of each configuration. It could be a mess if you forgive to check some things.

                                 

                                Hope it helps you.

                                 

                                Regards,

                            • Re: Configurations
                              Paul Risley

                              Since your workflow is heading in that direction already I would suggest using multi page drawings once you get the configurations handled. We do a lot of process drawings. 1 part multiple configurations multiple drawing sheets as you are starting to do. In the end it makes file management so much easier.

                                • Re: Configurations
                                  Chris Scougall

                                  Paul, I suggested that when I started working here a few months ago and the response I got was that they wanted to keep separate operation drawings so it would be "idiot proof" ( I know, poor phrasing) for the manufacturing floor folks. and I can understand that on some level.

                                    • Re: Configurations
                                      Ignacio Vital

                                      Hi Chris,

                                       

                                      I think Paul is saying that you have all of the drawings for the same part in diferent sheets of the same xxx.slddrw.

                                       

                                      You can use one sheet for each operation, but these way you only have a file which contains all the drawings you need to print for the part.

                                       

                                      The workflow for the operators doesn't change but I think that for you it will be easier to manage this way the drawings.

                                       

                                      If you need to have a copy of each sheet separately, you can save each sheet in PDF without a problem.

                                       

                                      Regards,

                                      • Re: Configurations
                                        Glenn Schroeder

                                        Chris Scougall wrote:

                                         

                                        Paul, I suggested that when I started working here a few months ago and the response I got was that they wanted to keep separate operation drawings so it would be "idiot proof" ( I know, poor phrasing) for the manufacturing floor folks. and I can understand that on some level.

                                         

                                        It's not poor phrasing, just impossible to achieve.  Every time I think I have something idiot-proof someone else invents a better idiot.

                                        • Re: Configurations
                                          Paul Risley

                                          You can have multiple sheets 1 file:

                                          Capture.JPG

                                          Each operation for this part has it's own drawing. But there is only 1 drawing file. You can name the drawing sheets whatever you want to and even put in header links that will produce the "drawing name" on the sheet. It works well for parts that need operational control. This part here has several profile grinds and each one needs to be detailed yet maintain controls on profiles already created. There used to be just 1 drawing with all of the details on it. When you factor in roll pins for inspection and all compound angles/ radii plus the need for validation inspections to happen it was a print that had 70 to 80 dimensions and controls on it. It was very busy.

                                            • Re: Configurations
                                              Chris Scougall

                                              I like this idea! I am going to push the managers for it. Since I can create a separate pdf file for each operation, I think they might go for it.

                                               

                                              Some operations require multiple sheets themselves, do you think that would be a problem?

                                                • Re: Configurations
                                                  Paul Risley

                                                  Chris Scougall wrote:

                                                   

                                                  I like this idea! I am going to push the managers for it. Since I can create a separate pdf file for each operation, I think they might go for it.

                                                   

                                                  Some operations require multiple sheets themselves, do you think that would be a problem?

                                                  Standards and organization will set up the operations with multiple step not being a problem. What I mean is how you set up the approach for handling these will determine if it is a problem or not. I would recommend playing with 1 part that has these multiple drawings and seeing what looks like it will work and what doesn't. Once you have it figured it out I would highly recommend setting up a template for just multiple sheet drawings we use 4 different templates for 4 different kinds of multi sheet drawings. (Notes and other things on the templates can be modified to suit your needs)

                                                   

                                                  It takes a little getting used to, but once in place you will wonder how you ever got along without doing it. Prime example for you and your situation. Take your stock part and make a drawing of it. Basic dimensions and whatnot. Right click in paper space, select copy and then select paste. Now you have a copy of your first page. Click on the model on the second page change it's configuration to the second op, detail the changes you need effected and move on to the next drawing page.

                                                   

                                                  It works well, but you need to establish some standards so that every one is on the same page.

                                                    • Re: Configurations
                                                      Chris Scougall

                                                      This sounds like some great advice. what I am struggling with right now on a practice model is I created a a model configuration for the first operation and then added a new configuration for the 2nd op. I thought I was careful setting all of the dimension to it's current config only but it didn't seem to work. the features for the 2nd op are being reflected on the first op. kind of frustrating