11 Replies Latest reply on Apr 10, 2014 10:52 AM by Sean Powell

    Q: rerouting all children from 1 datum plane to another.

    Sean Powell

      Hello, New to the forums here. If this is the wrong location hopefully a moderater will move it.

       

      This should be a simple question. For complex reasons the previous owner of a model created "Plane 2" offset from "Right" by 1 inch. That made sense when the part was conceptualized and 'right' matched with certain features in the assembly. Through successive iterations, all references to "Right" have been removed and features are now sketched on "Plane 2" or other surfaces and use "Plane 2" as a datum for dimensions. There are maybe 150 child features involved. There is no longer a practical reason to have a "Plane 2" and it currently overlaps "Right". The ideal would be to re-route all children from "Plane 2" to "Right" without manually fixing all of them individually. Solidworks 2014 Premium x64 now has a nifty "Replace Entity" function while sketching but I can't seem to find a replace or reroute for whole features.

       

      This should be as easy as:

       

      Replace

      Right

      Plane 2

      Done (<-- Can you see the ProE experience)

       

      I can't seem to find an appropriate command in Solidworks. Can anyone help?

       

      Thanks,

      Sean

        • Re: Q: rerouting all children from 1 datum plane to another.
          Jeremy Feist

          I don't believe this can be done globally in SW - I am pretty sure you would have to edit each feature/sketch to change its reference.

            • Re: Q: rerouting all children from 1 datum plane to another.
              Sean Powell

              Jeremy,


              Thank you and I'm assuming this to be true but hoping a more experienced Solidworks user might know something else or have a work around.

               

               

              My original experience with Solidworks in 2000 was that the interface was cute but functionality was limited. Coming back to it 14 years later it is apparantly the ProE can upgrade their interface easily but Solidworks seems to lack certain basic functionality that should be inherant in feature based solid modeling. I continuously encounter models with 'poor style' from my co-workers but further research indicates that fixing them is unreasonable based on limits of the software.

               

              Thank you

              Sean

                • Re: Q: rerouting all children from 1 datum plane to another.
                  John Burrill

                  Sean, without stepping into the API-which is a good idea if you have to do this conditioning a lot-the only path is to start at the bottom of the feature manager tree and work your way up replacing the reference.

                  You'll probably spend a lot less time making the plane useful then you will trying to replace it.

                  What are some UI upgrades present in ProE that you woudl like to see in SolidWorks?

                    • Re: Q: rerouting all children from 1 datum plane to another.
                      Sean Powell

                      "What are some UI upgrades present in ProE that you woudl like to see in SolidWorks?"

                       

                      John,

                      There are a few UI interfaces that drive me completely bonkers but most of my issues are functionality. There are 3 major UI interface upgrades that I would like see or to be shown where they already exist.

                       

                       

                      First, I have a perfectly good model tree scrolled to the middle of a 200+ feature part that I am modifying. I select a face and enter sketch mode or redefine a feature and my perfectly useful model tree is replaced with a feature creation menu and the tree is a collapsed ghost that overlaps my model where I must now expand and scroll and hunt for the named axis or other part of the model that I was just staring at 2 clicks earlier.

                       

                       

                      Second, The 'select other' function is clumsy and slow. If I have a shaft inside of a hollow cylinder and want to select the surface of the inner shaft takes too much fussing even with the swipe commands. In ProE a right-click would scroll through surfaces, edges etc in the selection spot and unigraphics the mouse wheel scrolls forward and back through that same selection. Quick and intuitive. I spend too much time repositioning assemblies so I can see the correct spot and not enough time doing the work with those selections.

                       

                       

                      Second-point-five. I have a lot of nested components in my assemblies so I frequently use transparent parts. Just because a part is transparent doesn't mean I am trying to select past it.

                       

                      Third: In a sketch why is the mouse hilighted with the 'create dimensions' icon when you are selecting dimensions to delete them? When dimensioning a sketch if a new dimension would cause a conflict with a constraint I need to drop out of the newly created dimension, loose the dimensioning tool, select the correct constraint, delete it and move back into the dimensioning tool. It is a tedious amount of mouse-pics that is much faster and cleaner in ProE.

                       

                      The rest of it really is engine functionality like replace, re-route, suppress without suppressing children (put them into failure mode as if the parent were deleted), poor capabilities to select silouete edges and an insistance on aligning sketches to edges rather than surfaces making sketches much more dependent on later features thus preventing efficient reordering.

                        • Re: Q: rerouting all children from 1 datum plane to another.
                          Glenn Schroeder

                          Sean Powell wrote:

                           

                          "What are some UI upgrades present in ProE that you woudl like to see in SolidWorks?"

                           

                           

                          Second-point-five. I have a lot of nested components in my assemblies so I frequently use transparent parts. Just because a part is transparent doesn't mean I am trying to select past it.

                           

                           

                          This one I can help with.  I just learned this recently, but if you hold Shift down you can select the outer transparent part or body instead of the part or body that's behind or inside it.

                            • Re: Q: rerouting all children from 1 datum plane to another.
                              Sean Powell

                              Glenn Schroeder wrote:

                               

                              This one I can help with.  I just learned this recently, but if you hold Shift down you can select the outer transparent part or body instead of the part or body that's behind or inside it.

                               

                               

                              Spectacular. I'll use that. Is there a good way to select the INSIDE surface of a hollow transparent part? IE selecting the c-bore of a bolt hole in a transparent engine block when the transmission housing is in the way of a direct select.

                               

                              Sean

                            • Re: Q: rerouting all children from 1 datum plane to another.
                              John Burrill

                              Sean, your perfectly good model tree is still there when you create a sketch entity-or select one.  Pick on the Feature Manager tab and it will display.  The creation menu is called the "Property Manager" and the Ghost menu you referred to is there so that you can select items from the tree while you're editing a feature like Extrude or Revolve.  I know Wildfire places this interface under the field of drawing

                              You have some options for changing the arrangement and display of the Feature Manager.

                              1. You can first turn off the automatic display of the property manager in the sketch by going into Tools>>Options: System Options tab: General panel and uncheck "Auto-show Property Manager".  The property manager options are still there, you just have to pick on the tab to show them
                                1. SW_manager_ui_config1.png
                              2. You can tear off the Property Manager Tab and dock it adjacent to the feature manager (or on the right-hand margin or on another monitor).  With "Autoshow Property Manager" turned off the dialog is hidden until you start a sketch command or select a sketch entity.
                                1. fm_manager_config3.png
                              3. You can split the Feature manager area and display the Feature Manager below the Property Manager
                                1. fm_manager_config4.png
                              4. The Ghost Menu-called the Flyout Property Manager can be displayed with an Opaque background. 
                                1. fm_manager_config5.png
                                2. fm_manager_config6.png
                              • Re: Q: rerouting all children from 1 datum plane to another.
                                John Burrill

                                Regaurding point 2: SolidWorks does reserve the mouse-wheel exclusively for zooming.  I know Inventor has the select through scrolling that you described.  One thing that might make the experience more fluid: Once you start the Select Other Tool (and I wish it was available as a hotkey or mousebutton assignment) you can drill down by right-clicking over any face to hide it.  You can even rotate the view with those faces hidden to get a better angle.  The display will persist like that until you do one of the following: left click in an empty area of the field of view, select a face or dismiss the "Select Other" dialog

                                SW_select_other_rmb.png

                                The Isolate command is useful If you want to temporarily hide everything besides the assembly components or part bodies you select in order to make working them easier.

                                sw_isolate.png

                                SW_isolate2.png

                                The "Exit" button in the dialog that pops up will return you to your previous display state (even if you turn on a part that's hidden)

                                • Re: Q: rerouting all children from 1 datum plane to another.
                                  John Burrill

                                  Point 3:

                                  I can The fact that the mouse displaying the same icon for creating a dimension as it does for selecting an might seem illogical-especially when SolidWorks goes to the trouble of displaying a pencil icon instead of the selection arrow for drawing something like a rectangle or circle.  I haven't thought about it extensively, but one reason they use a selection arrow might be that the smart dimension requires you to select entities to construct the dimension instead of specifying coordinates.  You can't create a dimension between arbitrary points in SolidWorks without placing points there, so there might be some insight there.

                                  • Re: Q: rerouting all children from 1 datum plane to another.
                                    John Burrill

                                    Your remarks on functionality all make good arguments.  You should submit those as enhancement requests.

                                    At the time of your posting, I had already drafted an enhancement request to allow dimensiong between 2D sketch entities and surfaces normal to the sketch plane to acheive the kind of robustness you described.

                                    There is the intersection curve sketch entity which can allow you to dimension to a face, but it only works if the face actually intersects the sketch plane and the relation once broken, can't be restored.

                                    I don't know if you know, but with convert entitities, you can also select a face to project onto a sketch and if the boundary of the face changes, the sketch will update.  This also works for the offset sketch tool.

                                    SW_Offset_sketch.png