6 Replies Latest reply on Jun 9, 2017 1:53 PM by Dan Pihlaja

    Hole callout not recognizing sketch driven pattern?

    Adam Dumm

      I like to create non-symmetric or irregular hole patterns using the sketch pattern feature. Works great in the part file and speeds up fastener mating using the pattern driven component pattern in assemblies. Yet when I go to detail the part or assembly I do not get the hole quantity with the hole callout tool??  Any ideas as to why SW can't add this like a normal linear or circular pattern?

        • Re: Hole callout not recognizing sketch driven pattern?
          Bjorn Hulman

          Hi Adam,

          when you use the hole wizard, it allows you to add all the points within the feature, basically creating a sketch driven pattern (if you expand out a hole wizard feature you'll find 2 sketches, one being the hole profile, the other the locations.)

          If you create you sketch within the hole wizard feature, it will give you the instance count in the hole callout. You can use a hole wizard feature to create a pattern driven pattern in assemblies.

            • Re: Hole callout not recognizing sketch driven pattern?
              Adam Dumm

              Thanks Bjorn!

              This is another option that does get the job done! The only down side is I have to go to the feature tree to get the sketch selected for patterning. Not the end of the world...but another click and then you also have to select the seed position. But an upside is it reduces a feature in the part and/or assembly. I will be sure to share with my team!

               

              Thanks,

              Adam

                • Re: Hole callout not recognizing sketch driven pattern?
                  Bjorn Hulman

                  At which point do you need to use the sketch of the hole wizard to create a pattern? to create a pattern in the part file? In the assembly a pattern driven pattern will allow you to select any hole from the hole wizard feature.

                   

                  I'm probably missing something here.

                    • Re: Hole callout not recognizing sketch driven pattern?
                      Adam Dumm

                      You're right, its just the seed position to worry about. I was playing with sketch driven pattern also. Thanks

                      • Re: Hole callout not recognizing sketch driven pattern?
                        Dan Pihlaja

                        Bjorn Hulman wrote:

                         

                        At which point do you need to use the sketch of the hole wizard to create a pattern? to create a pattern in the part file? In the assembly a pattern driven pattern will allow you to select any hole from the hole wizard feature.

                         

                        I'm probably missing something here.

                         

                        This is what I was doing:

                        In my skeleton sketch, I create a sketch with 1 circle (representing the first hole) and a bunch of points (representing the rest of the holes).

                         

                        Then, when I am modifying the part, I add the first hole and make the point concentric with the circle in the skeleton sketch.  I then exit the hole wizard and create a sketch driven pattern of the hole that I just created and select the same sketch I just used to align the hole.

                         

                        The reason that I do this, is that during the prototyping phase, I tend to delete and add holes to assemblies.  Before skeleton sketch, I would delete the holes on the first part, then have to go through each  part and delete the corresponding alignment holes.  Then at the assembly, would have to delete the bolts (or whatever) was in those holes that I deleted.

                         

                        NOW, with the sketch driven pattern, at the part level, for all the aligning holes I use the same sketch from the skeleton sketch for the sketch driven pattern for each part

                        Then at the assembly level I place the first component into the hole that is aligned with the circle in the first step and then use "pattern driven component pattern" to place the rest of the components.

                         

                        This way, when I have to change the number of holes, or add any holes, I just add them to the skeleton sketch and it updates all holes of all parts that align with those holes, and even quantities of the components at the assembly level.  It is working great!  Except for the count of the holes on the part level of the print.  That is the ONLY place that I am having a problem.  It is relatively minor, because I can just add it manually and move on, but it would be nice if it worked.