16 Replies Latest reply on May 8, 2017 9:25 AM by Jeremy Feist

    Strange Phantom line in part, also shows in drawing. ??

    David Shealey

      I have a part we inherited, made some changes, but it has a strange line in it that I cannot find the source of, and it shows up on the part and in the drawing.

      The 0.005mm extruded cut on each end is only to allow us to change the surface colors to match the part requirement.

      If anyone can find out where this strange line comes from, and how to get rid of it, it would be greatly appreciated. It is in SW 2016.

        • Re: Strange Phantom line in part, also shows in drawing. ??
          David Shealey

          The strange line is the vertical one in the left circular area.

          • Re: Strange Phantom line in part, also shows in drawing. ??
            Dan Pihlaja

            FYI, you don't need to make a .005 mm cut to split surfaces.....you can use the split line function to do that.

             

             

            It will create 2 (or more) surfaces where there was previously 1.  And then you can assign colors to each surface.

              • Re: Strange Phantom line in part, also shows in drawing. ??
                David Shealey

                That did it!  Now I have the proper color, and the phantom line is gone!  Thanks.

                Still learning SW, after decades of solid modeling in Solid Edge and Inventor.  SW seems to be far more difficult to become reasonably proficient in.

                  • Re: Strange Phantom line in part, also shows in drawing. ??
                    Jim Sculley

                    The line was being caused by a weird interaction due to the sheet metal part, your cut depth and the countersink edge here:

                     

                    If the depth in increased, the problem goes away at some point.  If the countersink is moved so that it doesn't intersect the cut, the problem goes away.  But most importantly, if you turn off the 'Normal Cut' option in the property manager for Cut-Extrude6 the problem goes away.  Another thread about a problem due to 'Normal Cut' can be found here: cut doesn't cut on both sides.  This is all academic however, since the correct answer is the split line solution.

                     

                    And now for some constructive criticism!

                     

                    Whenever I work on a model from a co-worker who has done this:

                    I become this guy:

                    Image result for anger pixar

                    All of the geometry and relations can be created in Sketch28 directly.  There is no need to sketch all the hole locations and then make a new sketch in the hole wizard that is all of those same locations again.  You end up with the Sketch just floating there in the feature tree not absorbed by any feature, with no clear indication about its intent.  Especially if the part has multiple hole wizard holes of the same size.  That sketch can be dragged all over the feature tree and quickly become lost relative to the hole wizard hole. When someone comes along later and wants to edit the hole wizard hole, they right click, select 'Edit Definition', click on the 'Positions' tab and are greeted by  a bunch of points with no relations, dimensions, etc.

                      • Re: Strange Phantom line in part, also shows in drawing. ??
                        David Shealey

                        Jim:

                        Regarding the extra sketch, that is something we did not do ourselves, when we put a sketch in, then use it to put holes in using the Hole Wizard, the additional sketch (plus the sketch that defines the hole itself) is added automatically.  We have been scratching our heads thinking this was a dumb thing, as Inventor does not do that.  In Inventor, we use a sketch, then put whatever holes we need in using that sketch.  It does not create another one.  We just assumed SW did that, and could not reason why it did.

                         

                        What procedure do you use that avoids the extra sketch? We would love to avoid it.  Hope you do not have to activate the Hole Wizard, THEN create the sketch inside the Hole Wizard tool.  We very often create a sketch knowing something is going to use it later, may not yet be ready to determine just what the hole is going to be.

                        • Re: Strange Phantom line in part, also shows in drawing. ??
                          John Stoltzfus

                          So what you do is add dimensions and relations in the HoleWizard 3D or 2D sketch?? 

                           

                          Here I use a controlling sketch just for the HoleWizard features and relate the point concentric to the sketch circles and the other relation is coincident with the face.. 

                           

                          So when you open up my files

                           

                          One sketch with multiple Holes or sometimes multiple sketches for one hole size

                           

                            • Re: Strange Phantom line in part, also shows in drawing. ??
                              Jim Sculley

                              John Stoltzfus wrote:

                               

                              So what you do is add dimensions and relations in the HoleWizard 3D or 2D sketch??

                              Yes.

                               

                              Here I use a controlling sketch just for the HoleWizard features and relate the point concentric to the sketch circles and the other relation is coincident with the face..

                               

                              So when you open up my files

                               

                              One sketch with multiple Holes or sometimes multiple sketches for one hole size

                               

                               

                              Let me just roll this model back and add 15 features between Shullenberg Holes and 3/8 Diameter Hole1.....

                               

                              Granted, the newish 'Dynamic Reference Visualization' is a vast improvement over the Parent/Child dialog, but I would rather my sketches be absorbed by my features.  It's too bad that HW holes couldn't work like lofts and the sketch would be absorbed.  Then everyone could be happy.

                                • Re: Strange Phantom line in part, also shows in drawing. ??
                                  David Shealey

                                  I would like to know how you get Hole Wizard to use a sketch that has been created, and  NOT have it automatically add an additional sketch!  Is there some setting we are not aware of?  That additional sketch has been driving us crazy.  We do not make it, SW does.

                                    • Re: Strange Phantom line in part, also shows in drawing. ??
                                      Jeremy Feist

                                      it is the first sketch that you created before the hole wizard that @Jim Sculley is calling "extra" - not the ones inside the hole wizard. we also work like Jim and do not use a sketch outside of the hole wizard.

                                       

                                      it is pretty easy to edit the hole wizard later if you determine you need a different hole size/type later, just show the location sketch in the tree so that any downstream relations can be added to the sketch element instead of the hole edges, as relations to those can break if you change hole types/options.

                                        • Re: Strange Phantom line in part, also shows in drawing. ??
                                          David Shealey

                                          After decades of using Solid Edge and Inventor, this just seems strange.  Will be hard to get into that mode of operation.  I prefer the Inventor way, put a sketch in that may be used for multiple operations, and use whatever we need from that sketch later to add needed holes.  sometimes we do not know what the final holes may be until later in the design. Do not want to have to re-create yet another sketch later in the Hole Wizard when the data could already be there.

                                           

                                          There are some things in SolidWorks I like, Exploded views are a little nicer. I like that they are configurations inside the assembly, not separate "Presentation" files as in Inventor.  However, Inventor puts the explode (tweak) lines in automatically if desired, do not have to add a explode line sketch later as in SW, which adds yet another step for drawing creation.

                                           

                                          Finding there is no "Wonderful" 3D modeling package, just some good ones. Moving from Solid Edge to Inventor was pretty easy. Inventor to SolidWorks, far more difficult.

                                        • Re: Strange Phantom line in part, also shows in drawing. ??
                                          Dan Pihlaja

                                          When you select the "positions" tab from the hole wizard, you are automatically entering a sketch.  You can either stop the point command that is automatically turned on and continue with your sketch, or drop a bunch of points and then come back later and edit the first sketch UNDER the hole wizard hole and add your relations.

                                        • Re: Strange Phantom line in part, also shows in drawing. ??
                                          John Stoltzfus

                                          I've had many more frustrations not doing a sketch first and since I have almost everything sketch driven it is much quicker.  Keep in mind that I'm only dealing with inserts and pins and some screw holes and an occasional through hole. 

                                           

                                          So for me I might have sketches on all 4 sides that get the same hole, I can tell you it is really nice just opening up the hole wizard once and select the positions on all sides, inside top bottom left right or on a weird plane... 

                                           

                                          It would be much much better for us if SW would consider using Hole Wizard information for "Smart Fasteners" till then the Smart Fastener is really dumb...

                                            • Re: Strange Phantom line in part, also shows in drawing. ??
                                              David Shealey

                                              Same for "Smart Mate". Would be great if it worked all the time, but it only works on some parts. Frustrating to use, as you never know if it will work.  We can always depend on the similar "Insert" command in Inventor to work as expected.

                                               

                                              If you think learning a new system is stressful, try moving back and forth between two! That is what a couple of us are doing almost daily here.  Often staring at the screen trying to remember where the needed command is.  8>)