12 Replies Latest reply on Jun 3, 2010 8:02 AM by Bill Stadler

    Better check your dimensions!

    Emilio Graff

      Here's a gem. Made me look like an idiot in front of a few people. Thanks. Makes you think twice about just sending drawings, doesn't it?

       

      nice_one.png 

        • Re: Better check your dimensions!
          Dwight Livingston

          I assume SW put in the diameter symbol, rather than it being added manually?

           

          And where is the R for the metric radius?

            • Re: Better check your dimensions!
              Emilio Graff

              If by "radius" you mean the distance to the flat, that's where the problem is---the dimension is completely wrong.

                • Re: Better check your dimensions!
                  Dwight Livingston

                  Emilio Graff wrote:

                   

                  If by "radius" you mean the distance to the flat, that's where the problem is---the dimension is completely wrong.

                  Okay, but it looks as if the 3.5" diameter dimension were a radius the distant to the flat would be proportionally correct.

                    • Re: Better check your dimensions!
                      Emilio Graff

                      It is not. The diameter symbol was inserted automatically, because if I just click on the round section of the part, SolidWaits defaults to selecting the dotted circle I drew on top of it. The circle has equal and concentric relations with the arc, and I also double-checked that this diameter dimension is correct.

                       

                      The problem is that the center mark inherited some random Z coordinate, which is of course not visible in a 2D drawing where the part is perfectly oriented in the XY plane, and because I selected "true" dimensions by ignoring the message SolidWaits is showing me the length of the hypotenuse of a triangle that I'm loooking at "head on".

                       

                      In other words, use projected dimensions even when you think true and projected should be equal, because SolidWaits is a mess.

                • Re: Better check your dimensions!
                  Wayne Tiffany

                  Is the view maybe set to real dims, not projected, and you got a point back in there somewhere?  Which one is correct?

                   

                    WT

                    • Re: Better check your dimensions!
                      Emilio Graff

                      Hmmm... can't remember. But I put in the view of the part, then tried dimensioning from the flat to the round part, and that didn't do anything. So I created a center mark with the round part, and dimensioned to that. Never thought twice about it. I then drew the dotted circle just for kicks. (I added its diameter to post here.)

                       

                      When I was told the dimension was "impossible", I opened the drawing, deleted the center mark, and dimensioned from the flat to the dotted circle, and that came out fine. I then also dimensioned the circle itself to ensure it was the same diameter as the round of the part (as shown here).

                        • Re: Better check your dimensions!
                          Emilio Graff

                          Wayne:

                           

                          I just checked; it was set to true dimensions. When I switch to projected, the centerline-to-flat dimension works.

                           

                          I don't understand why I even got asked about true/projected dimensions on this part; in the past, it's never made a difference (or so I thought). What is the point of "true" dimensions?

                            • Re: Better check your dimensions!
                              Wayne Tiffany

                              The point of true dims is generally for iso views where you want a real dim along a part that is not true to your view.  So if you drop the view in and it starts out as an iso view and it asks which you want and you don't pay any attention and you pick true and you then change to the front view you want and then you put your dims in,,,,,,,(I collected all the commas here...) then you can get a true dim in a view that is straight to you and still get attached to something that is back in the paper and things will not be right.

                               

                              So always pay attention to the messages that come up.

                               

                              WT

                              • Re: Better check your dimensions!
                                Jeremy Feist

                                true dimensions lets you properly show dimesions in isometric and other non-orthoganal views, where the projected distance between the lines of the part hold no direct meaning to the viewer.

                                 

                                Jeremy

                          • Re: Better check your dimensions!
                            Emilio Graff

                            It took a little "coaxing", but my VAR uncovered that this issue was previously reported as fixed, and now has been resuscitated.

                             

                            SPR #560253

                            • Re: Better check your dimensions!
                              Bill Stadler

                              We submitted something very similar not to long ago.  It cost us over a $1000 in rework not to mention the Engineering hours to chase down the issue and fix the drawings.  Talk about getting an earful from above.

                               

                              SPR's (Bugs)  SPR #: 332860

                               

                              Product:SolidWorks

                               

                              Status:Open

                               

                              Fixed in:none none

                              Area:Drawings

                               

                              Sub-Area:Drawing Views

                              Customer Impact:

                               

                              Summary:Dimensions default to 'True' when creating a Relative View - where Projected is required.

                              High

                               

                              Bill