15 Replies Latest reply on Sep 21, 2012 10:02 AM by Glenn Schroeder

    Just don't get it...

    Ryan McVay
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      9-18-2012 3-49-18 PM.png

      I had some free time today and decided to start playing around inside of SW 2011 MP5. I create a very simple part and I am attempting to cut a hole thru a portion of the solid.

       

      The solid is a simple extruded rectangle that has outside blends and then a hollow applied to it to create a structural tube.

       

      I now want to put a hole thru one side of the tube. The problem I’m having is that I cannot- for the life of me- get SW to allow me to locate the circle sketch from the edge or face of the exterior. I do NOT want to dimension off of the fillet. I’ve tried several different things and the only thing I could get to work was to place a plane on the planar face- which to me is redundant. I have even tried to convert the edge so that maybe I could use a point and even tried creating an intersection curve by selecting the two perpendicular faces..this really can’t be so!

       

       

      Why can’t I locate a hole from a face or edge? My design intent is to locate the hole from the mounting face- not a fillet tangency edge! I would like an answer based on deisgn intent not on part history. I know that I can reorder to get the results I want but that requires that I know where all my holes are prior to my actual design process!

       

      Frustrated….

        • Re: Just don't get it...
          Matt Lombard

          If you don't want to dimension from the fillets, then put your circle sketch before the fillet. If the fillet is in the sketch for the rectangular extrude, remove it and make them fillet features. Or you could show the sketch for the rectangle and dimension from the endpoint of one of the lines.

           

          I'm not defending the way it is, just trying to show how you can get where you want to go given the limitations of the process and your demands.

            • Re: Just don't get it...
              Ryan McVay

              Thanks Matt. My first attempts I was attempting to grab the sketch line and not the end point.

               

              So what causes me not to be able to position from a face but still allows me to select a plane on the same face? Don't both options provide me with a "intersecting" line on the sketch plane?

            • Re: Just don't get it...
              Dwight Livingston

              Ryan

               

              I don't understand why you don't want to dimension from the tangent. That is, after all, the edge of the side face.

               

              Dwight

                • Re: Just don't get it...
                  Ryan McVay

                  Dwight-

                  To your point- the edge that is "trimmed" back is also an edge on the same face.

                   

                  There are many reasons I don't like to dimension to tangents that are created by fillets. In this specific case, yes, the shape of the part is actually determined by the steel mill and the tangent/fillet isn't a problem.

                   

                  The primary reason I don't want to associate a feature with a tangency is that it keep my dependency structures as flat as possible which provides robustness in model changes. This way the hole, which is critical to the design, is only associated with tube/extruded face. Any changes to fillets don't cause or require the system to look at tangency. If I decide that I need to remove an edge from a fillet set I don't have to worry about the hole position failing. A failure could be critical to a design if that dimension is actually driving other parameters in your model. Keeping your structure as flat as possible and still maintain your design intent- I feel- is the best modeling practices out there.

                    • Re: Just don't get it...
                      Dwight Livingston

                      I understand about edits that will loose you your dimension. In many cases I try to start with a layout sketch or work with reference planes. Otherwise I just live with redimensioning.

                       

                      I would guess, even if you could dimension to a face, that when you did delete the fillets then the face ID would change and you'd loose the dimension anyway. Matt's advise is good.

                       

                      Dwight

                  • Re: Just don't get it...
                    Kelvin Lamport

                    You could use a 3D sketch (created on the face) to create the hole. That would allow the selection of a face when locating a dimension.

                     

                    Using the Hole Wizard allows the same.

                      • Re: Just don't get it...
                        Ryan McVay

                        It appears there a lot of different ways to skin this cat but the reality is that none of them outside of referencing the end point of the original sketch is the simpliest. Simpliest meaning the least complex with minimal amounts of click. Back to unlearning modeling using edges and feature relationships to keeping in mind that everything should be 2D/sketch based. Learning SW isn't the hard part. Unlearning 20+ years of 3D hybrid modeling is the hard part! I'm getting to old and stuborn...I want the system to work my way or not the systems way!

                      • Re: Just don't get it...
                        David Suelflow

                        Here’s how I would do it…

                        I try to sketch everything out in sketches at the top of the tree and relate everything to them.  As the design changes or evolves, I just go back to those sketches and make the changes there.

                         

                        Tube Hole.jpg

                         

                        • Re: Just don't get it...
                          Lenny Bucholz

                          holewiz with 3d sketch.jpg

                           

                          holewiz with 3d sketch-3.png

                           

                          Ryan,

                           

                          got your email at home and just saw it.

                           

                          I guess everyone out there forgets about "HOLEWIZARD"....................... use a 3d sketch and you can pick the faces to dimension too!!!!!!!!!!!!!!!!!!!!!!!!!!

                           

                          Message was edited by: Lenny Bucholz

                            • Re: Just don't get it...
                              Ryan McVay

                              @David-

                              Yeah, I'm not a fan of using offset curves in a sketch if it can be handled by a simple shell feature. I had the debate with one of our top users here this afternoon. My point was that you are having the system control and create extra entities and relationships that aren't necessary. His point was that I had three features doing what one could do. For me simplicity wins. That debate reminded me of training opportunity I had at an organization that was migrating from I-Deas to NX a couple years back. In I-Deas you tended to put as much information into the sketch as possible- as it was a more stable feature than having multiple features. The users were bring that logic forward on their current designs and their managers weren't seeing the improvements using the new software. I was invited in to do some migration training at that point. Needless to say we had to have a model throw-down between me and a couple of the users. Thankfully I won the throw-down. I won in both categories- the model design time and model modification. It wasn't such a hostile class after that. Some of the users actually thanked me for the challenge- they have been telling the old modeling SME's that for a month at that point.

                               

                              @Lenny-

                              @Kelvin-

                              Kelvin mention the 3D sketch but I couldn't find it during the extrude cut positioning. The hole wizard is were it was as you pointed out. So a "Thank you" goes out to both of you!

                              • Re: Just don't get it...
                                Kelvin Lamport

                                Kelvin mention the 3D sketch but I couldn't find it during the extrude cut positioning.

                                Start a 3D sketch, select a face (or vice versa), draw the sketch elements and then create the extrude-cut.

                              • Re: Just don't get it...
                                Glenn Schroeder

                                Ryan,

                                 

                                Maybe I'm missing something here, but you should be able to dimension from your hole to the outside face of the body.  I do it all the time.  Were you sketching with your model at an angle?  If that's the case, then it probably wouldn't work.  If your sketch plane is normal to your screen when placing the dimension then you should be able to select the outside edge of the body without a problem.

                                 

                                Glenn

                                 

                                Edit: 

                                I made a simple part to illustrate this but suddenly this morning I can't post models or screenshots. It hasn't been a problem until today.