24 Replies Latest reply on May 25, 2017 4:53 PM by Matt Gjertson

    Dangling dimensions/relations in edge flanges

    Matt Gjertson

      This post was inspired by this discussion.  This issue is described in SPRs 687261 and 837334, the latter was created for me on 11/11/2014 (the other one I simply found on my own).

       

      If I create an edge flange and dimension the length based of some other feature of the part, all is good.  That's parametric modeling, right?  Now, if I delete whatever feature is driving that edge flange, I see absolutely no indication that anything is wrong.  The feature manager does not show any warnings, and only if I go into the sketch of the edge flange do I see the dangling dimension.

       

      Dangling.png

       

      Anyone else experience this?  If so, do you have an open SPR for it?  If not, will you please vote on the two referenced above?

       

      Thanks

        • Re: Dangling dimensions/relations in edge flanges
          Scott Casale

          Your image shows a warning.  Could you show some more images to clarify when it doesn't show a warning?

          • Re: Dangling dimensions/relations in edge flanges
            Dan Pihlaja

            I want you to try something:

            Show your flat tree view, by RMB on the top and going to the above (I am in SW 2015, so maybe 2016 or 2017 has something slightly different).

             

            Then, while you are in flat tree view, run a CTRL Q and see where the error shows.

            • Re: Dangling dimensions/relations in edge flanges
              Matt Gjertson

              Here's another way to show the problem.  I created an edge flange on two edges.  I dimensioned the first one to 2" and I want the second one to be the same length so I make one of the lines equal to the corresponding line from the first flange profile.  Simple enough, right?

               

              Dangling-2a.png

               

              Now I go back and edit the definition of Edge-Flange1, deselect the first edge, then hit ok.  I just removed the entity that was being referenced by the second edge, which would make that equal relation dangling, right?

               

              Dangling-2b.png

               

              Now here's the best part, the relation doesn't even show as dangling!  Upon entering the sketch, everything looks fine and it looks fully defined.  The equal relation says it's referencing a sketch that no longer exists.  It doesn't even show up as brown like the dangling dimension from earlier did.

               

              Dangling-2c.png

               

              Does anyone else get this same behavior?  Does anyone get the expected warnings instead?

              • Re: Dangling dimensions/relations in edge flanges
                Michael Lord

                To add to the discussion.

                I would suggest that the reason you don't get a warning is that the sketch for the Edge Flange doesn't need to be fully defined, for the Edge Flange to be defined.  So although the dimension is dangling and was originally defining the distance of the Edge Flange, the Edge Flange is not effected by the dangling dimension.

                 

                You can see that if you try to edit the Edge Flange feature there is no dimension input box in the Flange Length.  If you delete the dangling dimension or the relationship (in the other example) the dimension input returns to the Edge Flange feature. 

                 

                I guess that is the nature of the sheet metal feature.  Should you get a warning, yes it would help!  Does it effect the model I would suggest not! 

                  • Re: Dangling dimensions/relations in edge flanges
                    Matt Gjertson

                    But then that's not consistent with the way everything else in SolidWorks works.  I just tried the same thing, but a little different.  I created an edge flange, and used "up to vertex" option (without editing the sketch profile).  Then I created an extrusion, up to the same vertex.  Next I rolled back the bar to before the flange and extrusion and made a cut to remove the vertex.  When I roll the bar forward the extrusion shows an error, but the flange does not.

                     

                    I beg to differ that it doesn't affect the model.  I have seen a few models of my own get screwed up because flanges are no longer updating properly, and can easily get left behind after making a few edits to the model.  That's actually how I noticed this a couple years ago.

                  • Re: Dangling dimensions/relations in edge flanges
                    Bernie Daraz

                    I think you have received the answer you were looking for so my comment is nothing more than a comment. I have extensive actual precision sheet metal fabrication experience so I model like I would actually 'build' the part in SW. I have received models with the the flange 'edited' within the sketch. It is quite frustrating to find that I cannot simply make the flange longer using the feature in the tree. Finding the flange holes and notches defined there is also an exercise in extra work as well.

                     

                    Mind you that I also mock up stuff in sheet metal and through the (sometimes) many edits I might make myself I do 'cheat' and cut down flanges using cut extrudes and move faces as well. But before I release that model to production I will redo it so it is a proper model and not the 'cluster f' that I finalized the prototype in before I release a production version. A model that is correct and flattens that could be imported as a DXF file into a programming system. Some newer systems like MetalSoft can import a SW model, there are others.

                      • Re: Dangling dimensions/relations in edge flanges
                        Matt Gjertson

                        Thanks Bernie.  I'd say that all just boils down to design intent then.  The stuff we make doesn't really fall into the "precision sheet metal" category, so I can understand treating each and every bend as its own entity in your case.  However, keep in mind that I also don't like "cheating" in modeling, and only used that specific method as an easy way to show the problem quickly and easily.  I've had this issue come up simply making a few edits to certain features in the model.  The way our parts work, there are only a few dimensions in the model that drive everything else, so I try to keep things related to each other as much as possible.  Edge-flanges are literally the only feature that don't let that happen, so it requires me to either disconnect them from the remaining dimensions (so they don't update at all when I modify the part) or leave them constrained to other entities, and just "know" when I need to fix them.  I don't like either of those workarounds as solutions, personally.

                          • Re: Dangling dimensions/relations in edge flanges
                            Bernie Daraz

                            Have you looked into Equations or in this sense constants?

                              • Re: Dangling dimensions/relations in edge flanges
                                Matt Gjertson

                                I use them when necessary for other things.  For this it just ends up being another workaround though, in my opinion.  If SolidWorks didn't acknowledge the problem exists, then I'd be more inclined to find a suitable workaround.

                                 

                                The most common way I do what I'm discussing is to make the floating edge of the edge-flange coincident to a point in a base sketch.  That's already done in many/most of my files, and I really don't want to have to go update all of them for a workaround.

                                  • Re: Dangling dimensions/relations in edge flanges
                                    Bernie Daraz

                                    Matt,

                                    I'm trying to understand the statement "The most common way I do what I'm discussing is to make the floating edge of the edge-flange coincident to a point in a base sketch." To me, the 'floating edge' is coincident to the base sketch by a dimension that is most often (every time for me) by the length of the flange. Of course that could change if inside material or tangent to radius (and other) dimensioning schemes are used. Of course I only use outside dimensions.

                                      • Re: Dangling dimensions/relations in edge flanges
                                        Matt Gjertson

                                        Like this:

                                         

                                        Dangling-3.png

                                         

                                        The base sketch, in this instance, is the sketch used for the main base-flange.  In a typical model (not all are exactly like this) there are only a few key dimensions, and most of the geometry of each model is resultant of those dimensions.  In this model, that point in Sketch1 would have a couple different flanges and maybe a few tabs that that use it as a reference.  Moving that point from 1" to 2" will drive all the other features that depend on it.  If I don't do it that way, then I have to manually go change each and ever feature instead.

                                         

                                        I know there are always many different ways to achieve the same sort of concepts, but this is how it's been chosen here.  It works very well for its intended purpose.  Almost every single new model here comes off of a different model (ie, open model A, change a dimension, save as model B).  This method makes creating new parts extremely quick and easy a vast majority of the time.  Occasionally, some of the edits are a little more extensive and end up breaking that chain.  It is only a problem when an edge-flange comes into play, which doesn't happen all that often.  That's what makes it so problematic to me though, since it's very easy to miss and end up cutting incorrect parts.

                                         

                                        We use a mix of "Material Inside" and "Material Outside" here for edge flanges, depending on what the end product is, but yes we always dimension to the outside for the brake operators.

                              • Re: Dangling dimensions/relations in edge flanges
                                Matt Gjertson

                                Just wanted to give an update to anyone interested.  My VAR received an Rx request from SolidWorks, which I happily supplied.  They changed the SPR to reflect that this problem is not file specific, saying that "there is a clear workflow to reproduce this issue."  Immediately following that, I was notified that this service call was "elevated to a Software Performance Report(SPR) and is now in the hands of the developers at SolidWorks."

                                 

                                Since this post was initially inspired by the fact that Steve Holland said the best way to get things fixed is to submit feedback in the Knowledge Base, if some of you guys would please go to the KB and submit feedback on SPR# 837334, I'd be very grateful if that helps get this fixed.

                                 

                                Thanks!