26 Replies Latest reply on May 27, 2010 10:22 AM by Eric Snyder

    Sketches that move with a part

    Eric Snyder

      I frequently make a solid and then sketches that are related to the solid with relations. Sometimes I want to move the solid (each move is associated with different configurations). The sketches have some relations to the solid but it is not fully defined. The sketches would take way longer to fully define. Using the automatic fully define slows things way down in the sketch.

       

      I want the sketch to move with the solid. I tried using a block which worked. The problem is that if you want to use the block to do operations like offset from those sketch entities then you have to explode the block, offset the entities and then make the block all over.

       

      Does anybody have a way to solve the problem of having a less than fully defined sketch move with a solid without making the sketch a block?

        • Re: Sketches that move with a part
          David Suelflow

          How about this…

           

          Make your solid and save it as a part.

          Do the "Make Assembly from Part".

          I usually "float" the part then mate it Top/Top, Right/Right & Front/Front.

           

          Do the Insert->Component->New Part and select the front plane.

          Exit the sketch without doing anything else.

          This will insert it at the origin with the proper Top/Top, Right/Right & Front/Front alignment.

           

          Start a new 3D Sketch and make it relate to the solid (or its sketch) in the original part.

          Save it internally or in a separate part file.

            • Re: Sketches that move with a part
              Eric Snyder

              You are basically saying to place the sketches in a seperate part in an assembly?

               

              Is it important to make the sketch a 3D sketch?

              • Re: Sketches that move with a part
                Eric Snyder
                Do the Insert->Component->New Part and select the front plane

                 

                The front plane of the part or the assembly?

                 

                I have tried this by creating a part (a rectangle) and then an assembly. I added a new part and added a couple of sketches. One sketch is an offset from some edges of the rectangle and is fully defined. The other is a partially defined sketch.

                 

                Then I edit the part (the rectangle) and add a configuration and do a move solid.

                 

                I then go back to the assembly and configure the rectangle part to the moved version and one sketch is fine but the other one "breaks". The fully defined sketch (the offset sketch) works fine. The second sketch gets messed up when the rectangle part gets moved to a different location using a configure component.

                 

                Attached is my attempt. What am I doing wrong?

              • Re: Sketches that move with a part
                Roland Schwarz

                When I need a "highly mobile" sketch, I start with a pair of perpendicular construction lines, then constrain everything to those construction lines.  Then I can move everything by moving a single point.

                 

                Even better if you start with your construction lines at an odd angle, eschew horizontal and vertical constraints, and use perpendicular and parallel to references, which will also allow you to rotate as well as translate.

                 

                For quickie constraints, you can use ordinate dimensions w.r.t. reference lines.

                  • Re: Sketches that move with a part
                    Eric Snyder

                    Interesting idea. My sketches unfortunatly usually have up to 100 - 200 arcs and lines. Defining all these manually to a single point would literally take hours. Using the automatically define option makes the skecth slow down considerably to the point where zooming a sketch just one click takes 2-3 seconds.

                      • Re: Sketches that move with a part
                        Lenny Bucholz

                        are you using the convert entity tool in sketch tool bar? if you aren't thats why it's taking you so long.

                          • Re: Sketches that move with a part
                            Eric Snyder

                            Typically I use "convert entity" to create a first sketch. The issue is that it creates the entities with splines. The splines need to be changed to lines and arcs to work well in production on a cnc machine. I create a second sketch and hand draw to create lines and arcs. The second sketch has some relationships to the first sketch but it is not completly defined. When I move the solid the first sketch (converted entities) moves just fine. The second sketch (not fully defined) does not.

                              • Re: Sketches that move with a part
                                David Suelflow

                                I don't like to use the convert entity if I can avoid it.  It always seems to slow things down detach more easily.

                                Anyway, attached is my fix with the second sketch fully defined without convert entities and an assembly configuration added.

                                  • Re: Sketches that move with a part
                                    Eric Snyder

                                    David:

                                     

                                    Thanks but I can't load it. I am using SW 2009 SP0.

                                      • Re: Sketches that move with a part
                                        Ryan Laplante

                                        Getting the sketches to move with the part is going to be diffucult -IMO-

                                         

                                        You can have multiple configs with a sketch for each part that is unique to the configuration.

                                        You need to have a configuration for each possible location the block can be in, this can be in the part view, the key is to suppress all but the active sketch in each configuration, and use the move copy bodies command to move the block and then add the new sketch just to that configuration, nothing should break at that point.

                                         

                                         

                                         

                                         

                                         

                                        This could be more easily done with Derived sketches and configurations, the derived sketch can be positioned and rotated just like the solid, using the copy/ mave bodies command on the solid - then rotating the sketch the exact same amount would keep everything aligned and if done if configs it couldn't break.

                                         

                                         

                                         

                                         

                                         

                                         

                                        Or look into advanced top down modeling using a part in an assembly that contains only sketches that drive parts and configs in other assemblies.

                                        • Re: Sketches that move with a part
                                          David Suelflow

                                          Doh!

                                           

                                          All I did was create an assembly configuration and configured the solid part to match (i.e. default/default & moved/moved).  Then I redid the second sketch to be a rectangle collinear with the first and with filets (with dims).  It was then fully defined and moved with the solid.  I'm not sure if you want to spend the time to do this for hundreds of line, I too am struggling with this.  Here's a shot of my assembly sketch…

                                      • Re: Sketches that move with a part
                                        Lenny Bucholz

                                        Eric,

                                         

                                        why are you wasting so much time making lines and arcs for the CNC? The reason I ask is because I am a machinist and cut straight from the SW solid in my CAM package (Surfcam) and can cut splines all day without any problems. What are you using to create your gcode? What CNC are you using? I have been using splines since 92 without a hitch and get great tool path.

                                         

                                        as with any underdefined blue sketch.....it has no smarts and doesn't have any links to tell it were to go. Why do you need it underdefined?