11 Replies Latest reply on Aug 9, 2017 12:14 PM by Paul Risley

    How do I get this to work?

    Eric Eubanks

      I'm trying to do this with the hinge and the door. SolidWorks How To Transfer Hole Location to Different Part in Assembly - YouTube

      I don't see the circles with the plus.

        • Re: How do I get this to work?
          Paul Risley

          Eric if you cannot get a relevant position from an existing hole to a different part(+) sign in the center of the hole to show up there could be a few things hindering that.

           

          First is under options making sure that the box marked"Do not create references external to the model" is not checked under system options>External references.

           

          The other possibility which is usually the culprit, the surface of the part you are putting holes into is not parallel to the part which you are trying to abstract the position from.

           

          Think of Solidworks this way if you have two plates stacked on top of each other you can drill through them with expected results. If the 2 plates are angled to each other one hole will not be a true circle, but an ellipse. Which will not be allowed by the software.

            • Re: How do I get this to work?
              Eric Eubanks

              "Do not create references external to the model" is not checked

              I moved the hinge away from the door using the triad so it should still be parallel.

                • Re: How do I get this to work?
                  Paul Risley

                  Eric,

                   

                  I did not load your model the other day. I just downloaded it now, what exactly are you struggling with as far as putting the holes in the cover with?

                   

                  I put them in and it works just fine.

                   

                  Edit the part you want the holes in while in assembly mode.

                   

                  Pick a face to put the holes in on the existing part.

                   

                  Put three holes anywhere you want then add a concentric relation to your #5 binding head holes and you are done.

                   

                  If you are waiting for the + to wake up you can do that and direct point to the holes as well.

                   

                  Either way works fine on your model.

              • Re: How do I get this to work?
                Christian Chu

                Eric,

                How can we open your assembly without any att. parts in it?

                • Re: How do I get this to work?
                  John Pesaturo

                  Edit the part you want to transfer the holes to within the assembly ...

                   

                  Create a sketch on said part / face ....

                   

                  Convert the entities from the part you wish to steal the hole locations from ...

                   

                  Edit: and voila ... Holes from one part to the next with an in-context edit if that's the right way to state it ...

                   

                  Second edit: I couldn't watch the YouTube video here (IT restrictions and all) so hopefully this is what you were trying to accomplish

                  • Re: How do I get this to work?
                    John Pesaturo

                    Eric, the only other thing I would note is that the location of your holes (Sketch 8, under CBORE for #5 Binding Head Machine Screw3) should be centralized on the hinge. Currently they are under defined and not symmetric.This will allow the same hole pattern to be used on both doors which should be the case as I'm sure you're only going to have one door designed but two used in the assembly.

                    • Re: How do I get this to work?
                      John Pesaturo

                      One more note ... If the "Convert Entities" does not allow you to pick the geometry you want to copy from you can also draw the three holes while editing the part. As long as the holes are drawn right on top of that hinge the holes will still be considered an "in-context" feature and should not require any dimensions to be fully defined (black). I had drawn the holes on the opposite side door using the hinge that was mated to it and it was there that I found the hole misalignment when I went back and looked at the opposite side.

                      • Re: How do I get this to work?
                        Todd Blacksher

                        Eric

                        It sounds as though you are talking about "waking up the center point" of an existing circle/feature -

                        As people have already mentioned, edit the part that you want the feature/sketch to appear on.

                        Next, you will need to "wake up" the center point

                        - this is the plus in the circle you mentioned

                        - The easiest way to do this is to hover over a circular edge, usually the quadrants work the best.

                        In the image above, I "hovered" my pointer over the counterbore on the hinge part on the right, the little line shows where my cursor was - in the yellow circle on the left, you can see the center point is now "awake" - at this point, you can move your cursor over to the plus in the circle, and click on it to place the circle with a relation to the center point of the hole on the hinge.

                        The center point might disappear when you move your mouse toward it, but when you get to the area where it is located, it should reappear.

                        At this angle it is a little harder to do, I recommend looking at it normal to the circle, so it is easier to see -

                        This is looking through the hinge to the mailbox.

                        todd

                          • Re: How do I get this to work?
                            Dan Pihlaja

                            Todd Blacksher wrote:

                             

                            Eric

                            It sounds as though you are talking about "waking up the center point" of an existing circle/feature -

                            As people have already mentioned, edit the part that you want the feature/sketch to appear on.

                            Next, you will need to "wake up" the center point

                            - this is the plus in the circle you mentioned

                            - The easiest way to do this is to hover over a circular edge, usually the quadrants work the best.

                            In the image above, I "hovered" my pointer over the counterbore on the hinge part on the right, the little line shows where my cursor was - in the yellow circle on the left, you can see the center point is now "awake" - at this point, you can move your cursor over to the plus in the circle, and click on it to place the circle with a relation to the center point of the hole on the hinge.

                            The center point might disappear when you move your mouse toward it, but when you get to the area where it is located, it should reappear.

                            At this angle it is a little harder to do, I recommend looking at it normal to the circle, so it is easier to see -

                            This is looking through the hinge to the mailbox.

                            todd

                             

                            Or you could use the sketch point from the sketch for the hole wizard hole.   Which might be more robust, because if you add a chamfer later or change the hole (say, from tapped to c'bored), that center point will need a new definition, while the sketch point will always be there unless you actually delete hole altogether.