13 Replies Latest reply on Dec 12, 2018 9:38 AM by David Matula

    hole suppressing

    Marek Petrzilka

      Hi all,

      it's a bit hard for me to explain exactly what I need to do....still I'll try:)

      I have a shaft with two holes created from one feature. Right now, in one configuration, I need to suppress one of them and in second configuration I need to have them both.

      I know that I can create them by extrude, pattern and for sure by many many more features:) So I don't need to know how to create them differently but I want to know, if there is possibility to suppress / unsupress multiple holes created by one hole wizard feature???? Inventor has this functionality and for me it was very useful.

       

      thanks

       

      marek

        • Re: hole suppressing
          Deepak Gupta

          Marek Petrzilka wrote:

           

          Inventor has this functionality and for me it was very useful.

          As far as I recall, you can do that only with a pattern feature/hole but not with holes created via one feature/sketch in Inventor. Can you show a video or link showcasing that feature. And if you really think that feature is worth then raise that as idea here SOLIDWORKS World 2019 Top Ten List

           

          And for SOLIDWORKS, you either need to create them as separate hole feature or pattern in order to suppress/unsuppress.

          • Re: hole suppressing
            Steve Calvert

            It's easy just to make the hole separate and control them that way.

             

            Steve C

            • Re: hole suppressing
              Glenn Schroeder

              As the others have said, you can't directly suppress one hole, but there is another simple option.  Use a Delete Face function to remove one of them, and suppress this feature in the configuration where you want both holes.

               

               

               

              • Re: hole suppressing
                Marek Petrzilka

                Deepak Gupta thanks for the advice, looks like pattern is the most suitable option for me. Luckily I need to control only two holes in this case..:D And from now on I know, that only extrude/pattern is the way of making holes, no more hole wizard:D

                 

                Glenn Schroeder try using my model and use deleteface to hole made by hole wizard not by extrude....it's not working, you just delete inner surface of the hole and make surface body from it and that is not solving my problem..

                 

                still, thank you for answers

                 

                marek

                  • Re: hole suppressing
                    Kevin Pymm

                    Marek,

                     

                    I have no problems using the Delete Face option (SW2019) & it doesn't create a surface body. Of course this option would become more complicated if your Hole Wizard holes were blind and/or CSK or Counterbored, as there would be other faces to pick.

                     

                     

                     

                    • Re: hole suppressing
                      Deepak Gupta

                      Marek Petrzilka wrote:

                       

                      Deepak Gupta thanks for the advice, looks like pattern is the most suitable option for me. Luckily I need to control only two holes in this case..:D And from now on I know, that only extrude/pattern is the way of making holes, no more hole wizard:D

                      You should definitely use hole wizard but for these kind of cases you can either use pattern or even create a new hole wizard feature.

                       

                      Also I'm curious to know as how it works in Inventor (in case it is different than what I mentioned above)

                        • Re: hole suppressing
                          Marek Petrzilka

                          IMO in Inventor the hole feature works much better than in Solidworks - based on my current experience of 11 years in Inventor, 4 months in Solidworks:)

                          And yes, it works as you wrote above via one feature/sketch. On the sketch you place crosses (representing hole axis) and by creating / editing hole feature you can select / unselect crosses from which you want to make a hole. Only if you need different sizes of the holes, you can use the same sketch but you need to create new hole feature with different diameter

                        • Re: hole suppressing
                          Steve Calvert

                          Let me explain my method.  One sketch to control location and then two (if you need them) hole features.  Sometimes we try and make things way more complex than need be.

                           

                          Steve C

                        • Re: hole suppressing
                          Kevin Chandler

                          Hello,

                           

                          If you can live with an error indication in the tree, you can do this using equations.

                           

                          I choose config 2 for what's shown below.

                          For the hole's 12mm location dimension, change it to this configuration.

                          Then create an equation that always moves it off the part. In this case, it's twice the overall length for this configuration.

                          Excessive, but guaranteed.

                          Default has two holes:

                          Config 2 has one hole and an error indication:

                          Each time you switch configs, this dialog is displayed:

                          As shown, you can dismiss it so it doesn't show again, but this will apply to all errors, intentional or not.

                           

                          I hope this helps.

                           

                          Kevin

                           

                          EDIT: Never mind. I just noticed it kills both holes of the feature.

                          • Re: hole suppressing
                            David Matula

                            to make things work for this situation I would have to make separate features for each hole. Just be sure to rename them so you know when you end up editing the part 6 months from now that you know which one is which.  Nothing like getting into a model that has many cut extrudes and not distention of where they are or what size they are.  I have been replacing them with hole cuts to reduce the features in the trees when I have the time.