9 Replies Latest reply on Mar 24, 2017 1:42 PM by Glenn Schroeder

    How can I "configuration-toggle" a mirrored cut-extrude ?

    Carmen Brown

      Here's what I want to end up with: a part with two configurations where Config A has the cut-out on the left. Config B has the cut-out on the right.

       

       

      The only way I could figure was to make two separate extrude-cut features, for the two configurations, and alternately suppress them.

      But this way means two sketches that must be updated separately.

      I'd like to combine the sketch and feature into a single entity.

       

      I tried several things, but came up for air empty handed.

        • Re: How can I "configuration-toggle" a mirrored cut-extrude ?
          Adam Hartles

          Carmen, how about a single sketch mirrored about a centreline so an update to one half changes the other.  Then 2 cut extrudes where you use the "Selected Contours" option to pick only one of the shapes. You'll have to expand Selected Contours within the property manager of the cut feature as it will default to being collapsed.

           

          Repeat for the other side and use the same suppres/unsuppress technique.

          • Re: How can I "configuration-toggle" a mirrored cut-extrude ?
            Glenn Schroeder

            Hello Carmen,

             

            Are those bodies mirrors of each other?  It looks like they are.  If that's the case, I'd model one, then create the second with the Mirror command.  Next delete the body of the first one (Insert > Features > Delete/Keep Body).  Now you have one body (the mirrored one).  Suppress the Mirror and Delete Body feature in the other configuration, so you have the original body for your second configuration.

              • Re: How can I "configuration-toggle" a mirrored cut-extrude ?
                Carmen Brown

                Hi Glenn,

                Thanks for the tip.

                "Delete/Keep Body" is new to me. The trouble is that it either wants to delete everything or nothing.

                 

                When I try to follow your suggestion to "delete the body of the first one" using "(Insert > Features > Delete/Keep Body)", how do I select just the part I want to delete?

                 

                 

                 

                 

                Here's what happened:

                In a part file, I made a block.

                 

                Then I cut a hole in the block.

                 

                Mirrored it.

                 

                 

                 

                 

                 

                 

                "Next delete the body of the first one (Insert > Features > Delete/Keep Body)."

                 

                I try to select the original cut-extrude by clicking in the hole shown by red arrow. But the entire block is selected, and it says that "mirror1" is selected. Anywhere I click on the part, it says "Mirror1" in "Bodies to delete"

                 

                 

                 

                 

                I click accept and get a totally deleted part.

                 

                 

                I select "Keep Bodies" and it keeps the whole thing.

                 

                 

                I tried to extrude a block from the main block and had similar results. It's all or nothing.

                I tried selecting the "Cut-Extrude" from the tree. It would not select.

                 

                How do I select "the body of the first one"?

              • Re: How can I "configuration-toggle" a mirrored cut-extrude ?
                Adam Hartles

                Carmen, you actually mirror the body (not the feature) and choose not to merge them- then you have two bodies over the top of one another. one a left hand one a right hand- then delete/keep body allows you to select accordingly.

                 

                Adam

                • Re: How can I "configuration-toggle" a mirrored cut-extrude ?
                  Scott Casale

                  Because SW 2017 has issues with using singular sketches for multiple features when selecting only some of the contours of the sketch used in individual features (such as what you have, 2 feature cut extrudes). The issue is that, if adjusting a parent item that the singular sketch is on (for a plane), the feature contour for each has to be re-selected.

                  Seen as:

                  1 sketch 2 individual cut extrudes

                   

                  What you could do is create a base sketch of the cut-out geometry, sketching for both sides.

                  Create an individual sketch with converted geometry for each in each sketch. Then extrude cut each sketch as desired.

                  When you need to update, just update the base sketch and both will be updated.

                  Seen as 1 base sketch

                  2 individual sketches

                  2 individual cut extrudes

                   

                  You could also create a base sketch of the cut-out geometry, sketching for both sides.

                  Create an individual sketch with converted geometry for one side, then extrude cut the one side from the individual sketch as desired.

                  Then mirror the cut extrude.

                  Seen as 1 Base sketch

                  1 individual sketch

                  1 individual cut extrude

                  1 mirror feature.