22 Replies Latest reply on Mar 14, 2019 4:58 PM by Henk Bruijn De

    What is wrong with this drawing?

    Paul Millhouse

      Hi all, I'm having a little bit of frustration with a drawing I made recently.

      I created a part then converted it to sheetmetal as you can see in the attached files.

      However some of the dimensions will not import and/or do not update on the drawing.

      Specifically my issues are as follows:

      1. Patterned hole callout (1/4" Clearance) model item will not import into drawing.
      2. Patterned & mirrored screw thread (1/4-20) model item not importing.
      3. Sheetmetal thickness won't import into drawing.
      4. I have altered the (sheetmetal) thickness and that is not reflected in the drawing. Had to override the value to get this drawing out.

       

      Basically every dimension that is shown as a reference (grey) wouldn't import although they are defined in the part.

      What is going on here? I imagine this is quite a simple fix but I can't seem to figure it out.

       

      Thanks

        • Re: What is wrong with this drawing?
          Henk Bruijn De

          Hi Paul Millhouse ,

          They grey dims are driven and have override checked. They should be driving dimensions without override checked.

          Replace the grey dims for new driving dimensions.

            • Re: What is wrong with this drawing?
              Paul Millhouse

              Hi Henk Bruijn De, thanks for the response.

              Yes I realize the grey dimensions are driven, I added them myself. I couldn't get the actual dimensions to import into the drawing using the Model Items button. Hence the question:

              How to get the actual driving dimensions to import correctly?

              What did you do to make that dimension show up as driving? Also that dimension should be 3/16" not 1/8"... It's been changed on the part but the drawing wouldn't update.

              Thanks

                • Re: What is wrong with this drawing?
                  Paul Millhouse

                  Okay I got the thickness dimension to import but the geometry still won't update.

                  As you can see the part itself does not correspond with the dimension lines... Can't figure out how to refresh that.

                  • Re: What is wrong with this drawing?
                    John Pesaturo

                    Paul, I'm not sure how to get your Boss Extrude thickness to auto populate in the drawing. It's not a feature that allows you to "Mark for Drawing" so unfortunately I can't be of any assistance there. You may have to simply manually place a dimension there to represent the thickness.

                     

                    I am however concerned about your thickness. You base extrude starts off at 3/16" (.1875") but when you get to your sheet metal conversion you have the thickness at 1/8" (.1250").

                     

                      • Re: What is wrong with this drawing?
                        Paul Millhouse

                        That did it, thanks. Changed the dimension in the Sheet-Metal conversion feature and it fixed the drawing as well.

                         

                        Still can't get my 1/4" clearance holes to auto-populate.

                          • Re: What is wrong with this drawing?
                            Newell Voss

                            Attach an image of your model items dialogue. I would assume you have items unchecked by your lack of hole location and pattern instance.

                              • Re: What is wrong with this drawing?
                                Paul Millhouse

                                Newell Voss, here you go.

                                SWX_callout_wont_import.png

                                 

                                I tried clicking various holes and got the same message every time ("No dimensions are inserted. The selected feature does not have dimensions.").

                                  • Re: What is wrong with this drawing?
                                    Newell Voss

                                    I would ensure you are specifying a layer, just as good practice. Also, if you switch to "entire model" in the source, does it yield different results?

                                    I have to assume you don't have "keep body" checked in the conversion feature?

                                    My guess is it has something to do with your workflow. When you create a model and then convert to sheet metal, it creates a new body which can sometimes lose feature details (ex: try adding a CS to one of your holes). If you start with a sheet metal feature at the top of your tree, all subsequent items should import as expected.

                                      • Re: What is wrong with this drawing?
                                        Paul Millhouse

                                        Same results if I have "entire model" or "selected feature" selected.

                                         

                                        Correct, I do not have "keep body" checked as I only want one of these things. My understanding is that you only "keep body" when you want to create a second (or third, etc) version using the same "base" (and that you would then uncheck "keep body" for the second one). Anyway, I wouldn't imagine that would have any impact on what I'm doing here.

                                         

                                        Okay, that makes sense. Unfortunately I'm unable to move the Convert-Solid feature up in the design chain. But if I Rollback and attempt to add a Convert to Sheet Metal feature earlier, then all subsequent features have errors because the edges defining the dimensions are lost. Another finicky SWX thing I guess. Anyway good to keep in mind for next time.

                              • Re: What is wrong with this drawing?
                                Henk Bruijn De

                                Hi Paul,

                                What did you do to make that dimension show up as driving?

                                I just added a new dimension, and it is driven by default.

                                 

                                If you want to import the dims in the drawing views automatically, there are some settings to check:

                                System options:

                                 

                                Document Properties (Drawing)

                                 

                                Hole callouts of patterned and mirrored holes is sometimes problematic.

                                I "workaround" in SW2018, by creating all hole positions in one sketch of the hole wizard feature.

                                Maybe SW2019 has improved this.

                                  • Re: What is wrong with this drawing?
                                    Paul Millhouse

                                    Henk Bruijn De wrote:

                                     

                                     

                                    Hole callouts of patterned and mirrored holes is sometimes problematic.

                                    I "workaround" in SW2018, by creating all hole positions in one sketch of the hole wizard feature.

                                    Maybe SW2019 has improved this.

                                    Can you please explain this a bit more?

                                    I did eventually get the dimensions to import using Model Items except for the patterned hole (which I agree is problematic).

                                     

                                    Also I generally avoid adding dimensions in the drawing, which always appear as reference dims for me. I prefer to import them directly from the part as driving dims.

                                      • Re: What is wrong with this drawing?
                                        Henk Bruijn De

                                        Hi Paul ,

                                        Can you please explain this a bit more?

                                        I did eventually get the dimensions to import using Model Items except for the patterned hole (which I agree is problematic).

                                        I just create 5 extra dots in your Sketch6 and suppress LPattern2 and Mirror1.

                                        Now all 6 holes are in on hole wizard Feature.

                                        In the Drawing I deleted your hole callout and put a new one in it.

                                        The new hole callout is still grey (I do not know why) but it updates well, including the nr of instances.

                                        The thread looks OK on all 6 holes.

                                        Also I generally avoid adding dimensions in the drawing, which always appear as reference dims for me. I prefer to import them directly from the part as driving dims.

                                        I usually apply all the dims manually in the drawing and take the risk I forget one. I think many users do It this way. It is also a matter of taste. 

                                          • Re: What is wrong with this drawing?
                                            Paul Millhouse

                                            Okay, I see. Nice trick haha. But, doing that defeats the purpose of using the pattern / mirror features.

                                             

                                            I got the 1/4-20 hole callout to import actually. It's the 1/4" clearance hole (patterned, not mirrored) that I could never get to import.

                                            It's the only one still in grey in the image below.

                                            PMT_Mounting_Shelf_Sheetmetal.PNG

                                            • Re: What is wrong with this drawing?
                                              Paul Millhouse

                                              I usually apply all the dims manually in the drawing and take the risk I forget one. I think many users do It this way. It is also a matter of taste.

                                              Yes, matter of preference. The way I see it, if the part is dimensioned and constrained properly, you shouldn't have to define anything in the drawing - they all just auto-import. I generally put a bit of thought into creating the part itself with this goal in mind. Makes my life easier in the long run. But when dims won't import I often add them manually just to get the drawing done.

                                                • Re: What is wrong with this drawing?
                                                  Henk Bruijn De

                                                  Hi Paul ,

                                                  I got the 1/4-20 hole callout to import actually. It's the 1/4" clearance hole (patterned, not mirrored) that I could never get to import.

                                                  Yes, this is also possible:

                                                  The pattern distance dimensions are Feature dimensions.

                                                  You have to checkmark the checkbox "include items from hidden features" (very cryptically description) for this, and than it imports automatically:

                                                    • Re: What is wrong with this drawing?
                                                      Paul Millhouse

                                                      Yes I did that. That's how I got the two 0.500" dimensions to import.

                                                      Again, it's the 1/4" clearance hole (0.266") that will not import no matter what I do.

                                                      It's the only one still in grey in the image I posted above.

                                                       

                                                      Thanks for your continued input though.

                                                        • Re: What is wrong with this drawing?
                                                          Henk Bruijn De

                                                          Hi Paul ,

                                                          it's the 1/4" clearance hole (0.266") that will not import no matter what I do.

                                                          Same thing happens to me with this one.

                                                            • Re: What is wrong with this drawing?
                                                              Paul Millhouse

                                                              It's either something with the patterning or something with the sheetmetal conversion. As far as I recall, patterned hole callouts will usually auto-import. Maybe converting it to sheetmetal has confused SWX somehow.

                                                                • Re: What is wrong with this drawing?
                                                                  Henk Bruijn De

                                                                  Hi Paul Millhouse ,

                                                                  Another attempt.

                                                                  As Newell Voss suggested, I started from the beginning with a sheet metal part and included the patterns and mirror.

                                                                  After automatic importing the dims in the drawing, it is still missing some dims of the 25-pattern hole, and the UNC threaded hole is twice mentioned.

                                                                  I accidently switched the "flat face", so the face with 6 holes is the "horizontal face" in my attempt.

                                                                  I think the problem is related to the holes and features in the "non-horziontal face" (in bended configuration).

                                                                  Interesting problem.

                                                                  Maybe the order of features can be a workaround.

                                                                    • Re: What is wrong with this drawing?
                                                                      Paul Millhouse

                                                                      Awesome! Thanks for doing that. I was going to attempt that myself, but I guess I don't have to, haha.

                                                                      I can live with a few added dimensions in my drawing. Still, curious why SWX does this.

                                                                        • Re: What is wrong with this drawing?
                                                                          Henk Bruijn De

                                                                          Hi Paul ,

                                                                          After my last posting I got the hunch that the sketch dimensions after bending are projected, and when automatically imported in the Drawing, SW ignores them because of that.

                                                                          So, if you want a flattened Drawing view, with all dimensions automatically imported, than you have to adjust your workflow.

                                                                          All holes and features must be created in the flattened position. You can create a Sketched bend after that.

                                                                          The result after auto arrange dims and some dragging:

                                                                          The 2,80 dim is the one of sketched bend, and is not neccesary in the flattened position.

                                                                          You can import the dims automatically for the Frontview also, but that does not make sense, because in that view you don't need so many dimensions. It seems that always some manually corrections are neccesary.

                                                                          Also the Auto Arrange functionality for dims has very limited usefulness.

                                                                          All these things makes me going on with applying all dims manually.