9 Replies Latest reply on Apr 30, 2012 2:23 PM by Jerry Steiger

    Colinear / horizontal relations issue

    William Grant

      Hello,

       

      I have a very simple brace part I am trying to add a dado to. I had originally made these parts within the assembly but when it came time to export the parts to my CAM program, I quickly realized that making the basic parts individually first then adding them to the assembly and finishing the design makes for a MUCH smoother export experience since everything is aligned correctly to the origin, etc...

       

      Onto my problem.

       

      I made this part individually using measured geometry of how the piece will fit in the assmebly instead of using a bunch of relations to other parts in the assembly. Thus, the part is square to its origin and all of the faces and edges are perpendicular to the default [front, right, top] sketch planes.

      BUT

      when I try to add a colinear relation to this last edge of the dado, it balks saying the horizontal relation causes a conflict. Now wait a minute SW, if I use the measure tool to check the two lines I am making colinear, "the two selected items are parallel".

       

      How does this make any sense? I don't want to just get rid of the horizontal relation and make a quick fix, because the line IS horizontal.

      If anyone has run into this before or has any suggestions on how to correct the issue I would be very thankful to learn from your experience.

       

       

       

       

      I tried to post some pictures (tried both jpg and png filetypes) but I kept receiving a database error. Hopefully everyone can open the [sw 2011] file.

        • Re: Colinear / horizontal relations issue
          Glenn Schroeder

          Your file didn't come through either. 

          • Re: Colinear / horizontal relations issue
            Scott McFadden

            William,

            I beleive you that your parts are parallel, but on the surface one might thing that there

            is a micro inch of difference between them.

            To add the images just RC in this open area and select "Insert Image"

            then browse to it.

            • Re: Colinear / horizontal relations issue
              William Grant

              Alright. I'm sorry guys but I think our corporate proxy is not letting me upload the files or something.

               

              So what do you suggest I do to more forward? Is it possible that the measure tool is limited by what sort of dimension precision I have set somewhre in settings?

               

              I used Measure to ensure all of the lines and planes were parallel to the original planes so I don't know which line or plane could be off.

                • Re: Colinear / horizontal relations issue
                  Scott McFadden

                  You might want to try and upload these outside of your office.  Say from home.

                  Email the images to your personal email and then upload them there.

                   

                   

                  Are you trying to upload them or insert them?

                  To upload are you using the advanced editor in the upper right corner or editing your last post

                  and at the bottom using the upload tool?

                  None of these are working for you?

                    • Re: Colinear / horizontal relations issue
                      William Grant

                      Yes I was using the advanced editor. When I attach a file at the bottom, it thinks for a while and says "unexpected error resulted". When I attach a picture using the insert image utility, it comes up with some com.blahblahblah errors saying the "put" method failed. Our network must be blocking document upload...

                       

                      Edit: I will upload the documents when I get home.

                       

                      Message was edited by: William Grant

                  • Re: Colinear / horizontal relations issue
                    David Suelflow

                    I have run into a similar/parallel issue… when I try to add a relation via the pop-up menu I will get a message saying that I cannot but if I click on the button on the FM it works.  It’s been doing this for years and I have been working around it but it would be nice if it could be fixed.

                    • Re: Colinear / horizontal relations issue
                      William Grant

                      Alright I did some more testing and I have some more info. I went into the Measure tool properties and manually set the precision to 8 significant figures. Then I worked my way from the origin planes to the line I am sketching.

                       

                      Bottom edge of part: orthogonal to all planes > the line I am trying to make my sketch line colinear to.

                      Sketch plane I am on: orthogonal to all planes. So my horizontal in the sketch plane shouldn't conflict with other horizontals.

                      Line I am attempting to relate to bottom edge: Parallel to bottom edge BEFORE I assign the colinear relation.

                       

                       

                      Summary: everything is fine before I apply the last relation, fully defining the sketch.

                       

                       

                      Now, when I apply the line colinear relation, there is introduced an angle between my line and the bottom edge of 0.00002417 degrees.

                      BUT!!! If I use a point coincident relation to make an point on the line touch the part edge that I want, then there is no problem. And there is no angle introduced.

                       

                      EDIT: There is no angle introduced but the whole line is some 0.000015 inches away from the part edge.

                       

                       

                      I no longer think it is a bug in the colinear mechanism, but rather a bug in using calculated geometry as a distance reference point...

                      I will post the file when I get home as a learning tool if anyone is still interested.

                       

                       

                      William

                       

                      Message was edited by: William Grant

                      • Re: Colinear / horizontal relations issue
                        William Grant

                        Here is how to fix the strange behavior:

                         

                        1. Go into Boss-Extrude > Sketch1

                        2. Make D2 less than 22.9808

                        3. Exit sketch and rebuild

                         

                        It seems I made a mistake in that my original part was slightly longer than the area it sits in. So when I extruded the end to the surface of the angle piece it buts up against it did something to the corner point I was referencing in Cut-Extrude3 to make it not lie on the edge line.

                        Then since I used that point as the reference for the geometry, the distance relation skewed the Sketch5 corner piece just a bit to force some angle.

                        It's been a long day figuring this one out...

                         

                        Cheers

                         

                        Message was edited by: William Grant

                          • Re: Colinear / horizontal relations issue
                            Jerry Steiger

                            William,

                             

                            You may have actually had a problem in your geometry, but I'm pretty sure that SolidWorks will get confused even if the underlying geometry is perfect. It just seems to get confused out there at the 8th place past the decimal piont in mm. The safest bet is to use the minimum number of degrees of freedom to drive your mates and relations. For instance, if you have two supposedly horizontal lines, you might want to dimension the distance between one line and the end point of the other line, rather than line to line. I usually get sloppy and  dimension between the two lines, only falling back to the line to point dimension when SolidWorks kicks up a fuss.

                             

                            Jerry Steiger