11 Replies Latest reply on Nov 27, 2013 10:33 AM by Deepak Gupta

    Separating Sketches?

    Nathan Reyburn

      Hello, I'm using Solidworks 2009-2010 and for some strange reason, recently, when I have gone to sketch two ellipses or two circles that have the same centrepoint, it classifies the two separate sketches as one individual sketch. I don't want this, because it won't let me to extrude one and extrude cut the other. So I want to know how to separate these two sketches into their individual parts, as I have not found a way to do it yet. Thank you.

        • Re: Separating Sketches?
          Glenn Schroeder

          Nathan,

           

          Welcome to the forum.  It's been a while since I used that version, but when you make the extruded boss or cut you should be able to choose which region of the sketch to use for the feature in the "Selected Contours" section of the PropertyManager (near the bottom).  I think it was there that far back but I'm not sure.

          • Re: Separating Sketches?
            J. Mather

            Attach the file here that exhibits this behavior.

            • Re: Separating Sketches?
              Jeff Holliday

              It is also possible to reuse the same sketch (or parts from it) in more than 1 feature (extrude/cut/etc).

              • Re: Separating Sketches?
                Deepak Gupta

                Welcome to SolidWorks forums Nathan.

                 

                As Glenn and Jeff suggested, you can use the selected contours option to select the area/entities for the features from a multi contour sketch.

                 

                Attached a simple video to show that

                 

                You might also find this post helpful for your future reference.

                • Re: Separating Sketches?
                  Lenny Bucholz

                  Nathan Reyburn wrote:

                   

                  Hello, I'm using Solidworks 2009-2010 and for some strange reason, recently, when I have gone to sketch two ellipses or two circles that have the same centrepoint, it classifies the two separate sketches as one individual sketch. I don't want this, because it won't let me to extrude one and extrude cut the other. So I want to know how to separate these two sketches into their individual parts, as I have not found a way to do it yet. Thank you.

                  Nathan,

                   

                  one sketch can only do one thing as a rule, extruded boss or cut, from the get go.

                   

                  so if you are saying you are making a dougnut sketch and you want to extrude to outer as a boss and the inner as a cut you would have to use the contour select tool at the bottom of the extrude property manager to the left, select the outer circle then extrude the exit.

                  Now click the + sign in front of the extrude feature, show the sketch select the sketch and now hit the extruded cut feature then click inside the small circle and then the cut property comes up and you can do a blind cut.

                   

                  or the simplest is just make to sketches for each feature...?

                   

                   

                  Selecting Contours

                  Select sketch contours and model edges, and apply features to them. This allows you to use a partial sketch to create features.

                  A tooltip appears when you cannot select a contour because:
                  • The part has too many edges.
                  • Edges are created on offset planes.
                  • Edges are chamfered.
                  • Edges are filleted.
                  Contour selection is also restricted as follows:
                  • When reusing a sketch, you can select only on the original face. If, for example, part of the face has been extruded, the tool does not recognize the new face.
                  • You can select contours only on the face with the sketch. If, for example, the face with the sketch is cut by a solid object (as shown below), the tool can select the part of the face still visible but does not recognize the solid object.
                    Contour_Select_Solid.gif
                  When creating lofts with 3D sketch contours as opposed to individual sketches, you can select one or more contours.

                   

                  To select and extrude contours:
                  1. In an active sketch, select a feature to apply the selected contours. For example, click one of the following to display the appropriate PropertyManager:
                    • Extruded Boss/Base Tool_Extruded_Boss_Base_Features.gif (Features toolbar)
                    • Revolved Boss/Base Tool_Revolved_Boss_Base_Features.gif (Features toolbar)
                    contour_select_sketch_00.gif
                  2. In the graphics area, use the pointer pointer_contour_select.gif to select a contour for Selected Contours

                    The contour can include model edges.

                    To select multiple contours, hold down Ctrl.

                     

                    contour_select_sketch_01.gifcontour_select_sketch_02.gif

                     

                     

                  3. Click PM_OK.gif to apply to the selected contours. 

                     


                    contour_select_sketch_03.gif

                    contour_select_sketch_04.gif
                    ExtrudeRevolve