8 Replies Latest reply on May 4, 2018 7:11 AM by Judy Wilson

    Creating part with multiple sketches

    Tom Hickerson

      I am experimenting with wire frame sketches to base my part creation and assemblies on.  So far things have been working pretty good.  However sometimes the wire frame sketches can become busy.  I tried creating multiple sketches with names of the parts they represent, and that is working good.  The problem is I can't select things between sketches like I can if it was all in one sketch. 

       

      In the example below the base frame sketch is the outer rectangle, and the inner rectangle is the moving slide.  I want to tie the midpoint of the base frame the the center-line of the moving slide.  It would not let me select the midpoint of the other sketch line.  It also won't let me dimension the length of the top like in base frame while editing moving slide so I could use equations. 

       

      So two questions....

      1.  Is there a better way to accomplish what I want keeping the wire frame sketch from getting cluttered?

      2.  How can I dimension and reference other sketches in a multiple sketch part?

       

       

       

       

        • Re: Creating part with multiple sketches
          Glenn Schroeder

          You should be able to insert a construction line and tie it to the midpoint of the inactive sketch, then link your active rectangle to this construction line with relations or dimensions, whichever is appropriate for your situation.

            • Re: Creating part with multiple sketches
              Tom Hickerson

              That does work. 

               

              One thing I can't do is dimension a line of the inactive sketch.  It will let me measure the line and show the dimension, but when I click it won't place the dimension.  Is there a way to make that work? 

                • Re: Creating part with multiple sketches
                  Glenn Schroeder

                  Tom Hickerson wrote:

                   

                  That does work.

                   

                  One thing I can't do is dimension a line of the inactive sketch. It will let me measure the line and show the dimension, but when I click it won't place the dimension. Is there a way to make that work?

                   

                  No, you can't dimension a line from an inactive sketch.  If you need that dimension for some reason in the active sketch then use the "Convert Entities" sketch tool to create a new line co-linear with it, and then you can insert a driven dimension on this line.  You'll probably need to change it to construction so it won't be used directly for an extrude, sweep,etc.

                    • Re: Creating part with multiple sketches
                      Judy Wilson

                      in answer to ?1 1.  Is there a better way to accomplish what I want keeping the wire frame sketch from getting cluttered?

                      Have you checked out display states?

                      use display states to show only the set of sketches you need at any time. It hides the portions of a sketch, or part, assembly that you do not need to see. Just name the display state with the grouping you need to work on.   ie all, moving slide, etc.

                       

                      in answer to your ? 2  How can I dimension and reference other sketches in a multiple sketch part

                      have you examined the skeleton sketch articles on this forum?

                      you seem to be heading down that road.

                      So,

                      a base sketch in which you have a set of points, the dimensioning and referencing is mainly done in the base sketch.

                      then, several other sketch's  which use  coincident relations to these points. thinking very carefully about and checking on any accidently auto relations established by SW.

                      for alignments of parts that do not work in the base sketch from the point level, try using planes dimensioned in the base sketch mated with a part face. Sketches based on those planes will move with the plane.

                        • Re: Creating part with multiple sketches
                          Tom Hickerson

                          I will check out display states.  It sounds like what I need for sure.

                           

                          Yes that is the road I am on.  I have read the articles and I am trying to fully utilize this methodology.  That last part of what you wrote has been my biggest struggle.  How to connect the other sketches to the base sketch.  Can you elaborate on the adding planes the the base sketch and creating a part on that plane?   I understand the concept, but how do you do that.  I see the plane in the base sketch, but how do you tie the part to that plane?

                            • Re: Creating part with multiple sketches
                              Judy Wilson

                              catch the planes.JPGeyeball.JPG

                              The concept rests on creating/building geometric relations between sketches/parts. this can be done using automatic relations or the display/delete relations command

                              These need to be built carefully, mindful of your end design goal.

                              For me, it helps to think of it as a pyramid structure. I forget it's correct name, but having the arrows(parent/child) point up and down the feature tree really helps at this point.

                              I have attached an example:Multisketch (using SW 2017)

                              The order of the layout of the feature tree is important. Here, the concept rests on the automatic insertion of relations by SW when you are drawing.

                               

                              The prep work before sketching the box.

                              Creating the planes TOP OF BOX, OTHER SIDE OF BOX.  These planes were created parallel to the main planes with reference to a sketch line. The sketch line is dimensioned from the origin. Here is where you control the location of the plane.

                               

                              In my box part below, when I sketched the rectangle in the FRONT plane, clicking the cursor when highlighting the TOP OF BOX plane and the TOP plane resulted in the above picture. Those lines are now coincident with the planes.

                              Move the planes, move the lines. This is one way the part can get tied to the plane.

                               

                              The side of box sketch gets extruded to the next surface which is the OTHER SIDE OF BOX PLANE. 

                              Voila, a controlled box

                               

                              This is why skeleton sketch is such a good name for the technique. As you move the base points, the rest of the structure follows.

                               

                               

                              Issues

                              if you run into an issue when you cannot drag an item in the feature tree above say a reference plane, but you need to. You likely have an inadvertent relation created that keeps the feature from moving.

                              The eyeball icon picture is where you can show / hide planes visible in the part.

                               

                              I added a set of display states to toggle through in the part. Display states does seem to be a quicker easier of running through different views of a part.

                                • Re: Creating part with multiple sketches
                                  Steven Mills

                                  Little tip, when I have to keep multiple dimensions related/referenced across multiple sketches and even features, I start using equations. Heck, you can have value "A" = 30, then right click on a dimension and link it to value "A". You can even reference other parts and assemblies through the equations tool. It can be simpler than trying to to manage a bunch of relations.

                                   

                                  Mind you, I generally find it easier to use equations, but that is just me.

                                    • Re: Creating part with multiple sketches
                                      Judy Wilson

                                      I also use equations frequently, but when i started using design tables, i found out equations and design tables do not play nice together.

                                      Now I am using Driveworks Xpress for some parts, i need to get rid of my equations and replace them with rules.

                                      But yes, I also find them useful to collect info in one spot.

                                       

                                      In Tom's case, he needs the relations to make the sketches follow the skeleton sketch. Then he could use equations to adjust the dimensions easily.