20 Replies Latest reply on May 14, 2018 9:04 AM by Glenn Schroeder

    Guiding dimensions

    Hugo Liano

      Hi,

       

      can anyone explain to me the difference between guiding dimensions and reference measurements? If I made a draw with guiding dimension how can I change it to the ref. measurements?

       

      Thanks.

        • Re: Guiding dimensions
          Glenn Schroeder

          I'm not familiar with the term "guiding dimension" either.  Can you explain the context where you saw or heard it?

          • Re: Guiding dimensions
            John Pesaturo

            Hugo, just in case it's this straight forward ...

             

            Changing a dimension to a "reference dimension" is as simple as clicking the highlighted toggle. You can also group select multiple dimensions and change them all at the same time by Ctrl selecting them and then clicking the toggle as well.

             

            • Re: Guiding dimensions
              Hugo Liano

              hi, all is because I make a course about CAD, my project was not ok because I had in the draw several driving measures

               

              IMG_0520.jpg

               

              the only my teacher said is:

               

              Captura de pantalla 2018-05-10 a la(s) 14.48.34.png

               

              I don't know if he meant only to tryck that but I´d like to know what´s the difference

                • Re: Guiding dimensions
                  Dan Pihlaja

                  What you are referencing in this picture is the "Toggle Color Display Mode" in a drawing.

                   

                  This shouldn't affect driving dimensions at all. 

                  • Re: Guiding dimensions
                    Dan Pihlaja

                    OK, nevermind....I think that I get it.

                     

                    I think that you are talking about the difference between these two dimensions:

                     

                    They are different color, which could be a difference between layer definitions or a difference between driven and driving.  Depending on where you toggle is at the moment

                     

                    I have a couple of questions about your drawing methods:

                    1) It looks to me like you are drawing in your centerlines by hand and then dimensioning them?   Is this true?  If so, you don't need to do that (generally).   You can use the centerline and center mark tools:

                     

                    2) OR are your different dimensions on different layers?

                     

                    That little toggle that you referenced just toggles between the layer definition (which is how it will print) and the system definition of things (which color codes things based on different criteria, giving you a good clue as to what type of item it is).

                    • Re: Guiding dimensions
                      J. Mather

                      There are three different issues/competencies that I would grade related to drawing standards.

                      But I would not communicate with poor quality pictures.

                      1. You can grab nice screen captures with the built-in Windows Snipping tool.

                      2. But I don't even like to fool with pretty pictures.  My response would be, "Why are you using CAD to design and then not using CAD to communicate?"

                      Attach your *.sldprt file and *.slddrw file and I will comment further.

                    • Re: Guiding dimensions
                      M. D.

                      As far as I can gather there are either "Driven" or "non-driven" dimensions.  I don't think it is thought of as driven or driving but I may be wrong.  A driven dimension is a dimension where Solidworks is telling you "That dimension won't actually work and your sketch is over constrained, but if you say so then we will display it"  A driven dimension (the grey ones) are basically impossible dimensions as far as other sketch constraints or relations are concerned.  so if it asks you "do you want to make this dimension driven?" that is a bad sign and always cancel.

                       

                      I guess normal dimensions are considered "driving".  Here is a good explanation:

                      Beginner question: What do the terms 'driven' and 'driving' mean?

                        • Re: Guiding dimensions
                          Kevin Chandler

                          Marcus Dimarco wrote:

                           

                          As far as I can gather there are either "Driven" or "non-driven" dimensions. I don't think it is thought of as driven or driving but I may be wrong. A driven dimension is a dimension where Solidworks is telling you "That dimension won't actually work and your sketch is over constrained, but if you say so then we will display it" A driven dimension (the grey ones) are basically impossible dimensions as far as other sketch constraints or relations are concerned. so if it asks you "do you want to make this dimension driven?" that is a bad sign and always cancel.

                           

                          I guess normal dimensions are considered "driving". Here is a good explanation:

                          Beginner question: What do the terms 'driven' and 'driving' mean?

                          Hello,

                           

                          I don't believe the presence of a driven dimension necessarily means your sketch is overconstrained.

                          A driven dimension is just an indication that that particular dimension is referring to geometry that's already resolved by other dimension(s), other geometric condition(s) or a combination of these.

                          It could be a simple case of a duplication of another sketch dimension.

                          Until the sketch is fully defined, other portions of the sketch are free to move regardless of driven dimensions.

                           

                          I also don't always consider a driven dimension a "bad" sign.

                          I sometimes add them to purposefully show a driven intent, to check that what I believe should be driven actually is driven and also to investigate the intent of a previous design to see if it is driven (and assess whether it should be or not).

                          They're handy to add when geometry is being resolved by the "invisible stuff" like relations (I don't run with them displayed). and you'd like a little eye candy to see how things are measuring up. If your sketch has few, if any, dims and a whole bunch of trig happening, add a driven dim (or two).

                          I've also created driven dimensions for use in cross-feature equation references.

                          When you create a global variable using the Measure option, you're creating a driven dimension.

                           

                          I "don't show me again" the driven dialog long ago with a yes to accept any and every driven dim.

                          If I create a boo-boo driven dim, I just delete it. And plod on.

                           

                          Like most of SW's bits, driven dims have their positive uses.

                           

                          Cheers,

                           

                          Kevin

                            • Re: Guiding dimensions
                              M. D.

                              Sure but in general when you see that dialog it is accompanied with a lot of red and yellow on the screen and generally you want to slowly back away .  Typically I don't like to use driven dimensions as reference dimensions since I make drawings, and I will just add in a dimension in the drawing itself if that dimension wasn't needed in the model to fully define it.  I don't think either way is inherently better but I'm curious how many people do it this way rather than use driven dimensions?

                               

                              Maybe Solidworks intends for us to use driven dimensions in this situation but for some reasons the "red and yellow warning" and the default different appearance of driven dimensions give us an aversion to it?

                                • Re: Guiding dimensions
                                  Glenn Schroeder

                                  Marcus Dimarco wrote:

                                   

                                  Sure but in general when you see that dialog it is accompanied with a lot of red and yellow on the screen and generally you want to slowly back away . Typically I don't like to use driven dimensions as reference dimensions since I make drawings, and I will just add in a dimension in the drawing itself if that dimension wasn't needed in the model to fully define it. I don't think either way is inherently better but I'm curious how many people do it this way rather than use driven dimensions?

                                   

                                  Maybe Solidworks intends for us to use driven dimensions in this situation but for some reasons the "red and yellow warning" and the default different appearance of driven dimensions give us an aversion to it?

                                   

                                  The setting below will eliminate all, or at least almost all, of the errors when adding a driven dimension.  And I, and many other users, don't use model items in Drawings at all, but instead insert all of them as needed manually with the Smart Dimension tool.  There have been a number of other Discussions here asking the same question.

                                   

                                    • Re: Guiding dimensions
                                      Steve Calvert

                                      Glenn, I use, and try to teach others to use, model dimensions as much as possible.  I seem to do more sheet metal than just about any other so that makes it a little more simple but I'll do the same for my plastic injection parts and cast parts.  Now having said all this, I'll for sure do a diligent enough of a job naming my features so I know what dims needed to be added in the end.

                                       

                                      I guess we all have our preferences...

                                       

                                      Steve C

                                        • Re: Guiding dimensions
                                          Glenn Schroeder

                                          Steve,

                                           

                                          I wouldn't argue with anyone that uses them, but for me when I was first getting started learning SW it just seemed that I had to spend so much time moving them around to look right that it was just easier to insert them myself.  Plus when I'm modeling I don't want to have to worry about how I'm going to dimension the Drawing.  And third, I have a number of dimensions in almost every that are showing Part locations in an Assembly, and as far as I know they'd have to be inserted manually anyway.

                                           

                                          Glenn