7 Replies Latest reply on Mar 28, 2018 2:48 PM by Glenn Schroeder

    Mirror section of part?

    Nelson Lopes

      I'm a newbie to Solidworks and this is my very first design.  I'm trying to create a bracket that I want to eventually save as an STL, slice it into gCode for a 3D printer.  I designed most of it and attached the Solidworks drawing file below.  This is supposed to have two (2) of the clamps on each side.  I created one and would like to "mirror" it to the other side, but cannot figure out how to do this for the life of me!  Not sure if I'm to mirror a feature, entity, etc. (don't know the differences between them).

       

      Hopefully I created the part correctly - I found myself sketching rectangles and extruding them, etc. to create the entire part - so it's sort of "in pieces" and don't know if I need to "merge" or "combine" them together.  Not sure how to do that either.  It turned out great though!  Any help and detailed instructions to correct this and mirror the "clip" to the other side would be greatly appreciated.  Love learning this!  Thank you very much!

       

      Kind Regards,

      Nelson

        • Re: Mirror section of part?
          Glenn Schroeder

          Welcome to SolidWorks, and this forum.  Many users won't open links.  Please attach your Part here and I'm sure we'll be able to help.  See How can I attach a file to a forum post? for directions.

            • Re: Mirror section of part?
              Tony Tieuli

              Nelson Lopes wrote:

               

              I'm a newbie to Solidworks and this is my very first design. I'm trying to create a bracket that I want to eventually save as an STL, slice it into gCode for a 3D printer. I designed most of it and below is the link to the Solidworks file (shared on Google Drive). This is supposed to have two (2) of the clamps on each side. I created one and would like to "mirror" it to the other side, but cannot figure out how to do this for the life of me! Not sure if I'm to mirror a feature, entity, etc. (don't know the differences between them).

               

              Hopefully I created the part correctly - I found myself sketching rectangles and extruding them, etc. to create the entire part - so it's sort of "in pieces" and don't know if I need to "merge" or "combine" them together. Not sure how to do that either. It turned out great though! Any help and detailed instructions to correct this and mirror the "clip" to the other side would be greatly appreciated. Love learning this! Thank you very much!

               

              New Bracket.2.SLDPRT - Google Drive

              Hi Nelson,

              Welcome to the forums!

              What you want to do is create a new reference plane in the center of your bracket and then mirror your clip around that plane.

              Make your new plane parallel to the right plane and select the midpoint of the bracket as the second reference.

               

              bracket.png

               

              Make sure you select all of the features you used to make your clip when you mirror it.

              You should get the result shown below.

               

              bracket 2.png

               

              Hope this helps.

            • Re: Mirror section of part?
              Nelson Lopes

              @Tony - Thank you!!  I was not aware of how to do the reference plane.  Just looked that up and was able to place it in the drawing and the mirroring was a piece of cake now!  Much appreciated!

               

              Kind Regards,

              Nelson

                • Re: Mirror section of part?
                  Tony Tieuli

                  Nelson Lopes wrote:

                   

                  @Tony - Thank you!! I was not aware of how to do the reference plane. Just looked that up and was able to place it in the drawing and the mirroring was a piece of cake now! Much appreciated!

                   

                  Kind Regards,

                  Nelson

                  You're very welcome.

                  Best of luck learning and using Solidworks!

                    • Re: Mirror section of part?
                      Nelson Lopes

                      @Tony - I do have a couple of questions regarding this first design of mine in SolidWorks. 

                       

                      1). Is it okay the way I created this using multiple rectangles to sketch/extrude it?  I believe it becomes all one part, but not sure if I need to combine/merge them somehow?  Or if that makes it better when creating an STL to slice into gCode for a 3D printer.

                       

                      2). When I created the reference plane as you suggested, I set it's offset by entering the measurement manually since I knew (center) of the base width.  Is there a way to automatically center the plane at a midpoint by simply selecting the line/part?  Still unfamiliar with all the tools/toolbars if this is possible.

                       

                      Best Regards,

                      Nelson

                        • Re: Mirror section of part?
                          Tony Tieuli

                          Nelson Lopes wrote:

                           

                          @Tony - I do have a couple of questions regarding this first design of mine in SolidWorks.

                           

                          1). Is it okay the way I created this using multiple rectangles to sketch/extrude it? I believe it becomes all one part, but not sure if I need to combine/merge them somehow? Or if that makes it better when creating an STL to slice into gCode for a 3D printer.

                           

                          2). When I created the reference plane as you suggested, I set it's offset by entering the measurement manually since I knew (center) of the base width. Is there a way to automatically center the plane at a midpoint by simply selecting the line/part? Still unfamiliar with all the tools/toolbars if this is possible.

                           

                          Best Regards,

                          Nelson

                          Nelson,

                          Your method is fine. You merged your features as you went along. No need for any other combine/merge.

                          I really can't speak to your question about the best method for creating a part that is to be 3D printed. I have no experience with that.

                           

                          You could have selected the midpoint on the bracket base to center the plane.

                          Take a look at the image below.

                           

                          bracket 3.png

                           

                          If you click inside of the Second Reference box then hover over the line where the purple spot is shown, the midpoint of the line will appear. Just click on that point and your new reference plane will be centered.

                          The method you used to place the plane is just as valid.

                          • Re: Mirror section of part?
                            Glenn Schroeder

                            Nelson,

                             

                            I'm not Tony, but I'll reply anyway if you don't mind.  There's really nothing wrong with the way you modeled this, but I'd have made it simpler if I was doing it.  I'd have created the part shown below with all one feature.

                             

                             

                            I'd have made a U-shaped sketch, and I'd have centered it on one of the main planes so later you could use it for the Mirror feature instead of needing to create a new one.  Using symmetry is one of the most important things you can learn when using SolidWorks.  First I'd have placed a construction line vertical from the origin (which will be used to dimension across, and later for mirroring sketch entities).  Next I'd sketch two lines in an L-shape and dimension them as shown below.  (I didn't use your dimensions; I like to keep things simple.)

                             

                             

                            Then use the Mirror Sketch Entities function to place them on the other side.

                             

                             

                             

                            Next, use the Offset Entities tool to finish the U shape, using the options shown below.

                             

                             

                             

                            Close out the sketch and extrude it.  By the way, I'd use the Midplane option instead of Blind so the plane that's perpendicular to your sketch plane would be centered on your body also.  Next, using the same technique you could create the clip with one feature, and since the part was started centered on a plane you can use the same plane to mirror it.

                             

                            Going back to your Part, if you want to keep going with what you have, creating the plane is really very simple.  Activate the Plane command, and then choose two faces (either the two inside faces of the U-shape, or the two outside faces).  That will place the plane midway between them.  There's nothing wrong with the way Tony Tieuli  suggested, but I prefer using the midplane option in the example you posted.

                             

                            Also, you mentioned combining the bodies.  You'll likely have better luck getting the Mirror feature to work by creating the clip as a separate body first,and then make sure to choose "Bodies to Mirror" ("Features to Mirror" will be selected by default) in the Property Manager when mirroring.  You can always use the Combine feature later to combine all bodies.