19 Replies Latest reply on Nov 11, 2009 4:54 PM by 1-4EQZK9

    hi everybody

    scott sides
      I imported a step file and the part is zoomed way out. Is there a way I can change the standard views so that the part is zoomed in closer.
        • Re: hi everybody
          Tony Cantrell
          Check to see if something is out in space, it should zoom to the part extents.
          • Re: hi everybody

            Scott,

             

            before you go any further, make sure that you imported it in the correct units.

             

            Regards

             

            Mark

              • Re: hi everybody
                scott sides
                model size checks ok
                  • Re: hi everybody
                    Charles Culp
                    try uploading the part again, only pull the actual file instead of the temp file.
                      • Re: hi everybody
                        scott sides
                        try this one
                          • Re: hi everybody
                            Matt Lombard
                            Yeah, that part is hosed. I can't put my finger on anything exactly wrong, but it has edges poking through, the display quality is really bad. Import Diagnosis is clean and so is Check. I jacked up the display quality settings, and SW hung. Do you have to original translation file?
                              • Re: hi everybody
                                scott sides
                                no thats all i have
                                • Re: hi everybody
                                  Jim Sculley

                                  I get a SW hang when moving the Image quality slider into the red zone as well.

                                   

                                  Some forensic analysis:

                                   

                                  A.  Cut away a quadrant of the model.  Zooming now behaves and display quality improves.  Delete or suppress this cut.  Problems return.

                                  B.  Sketch a circle on the flat underside of the part.  Position it over potential trouble spots (fillet intersections, tangent edges, etc..).  Extrude cut thru all , see if problems go away.

                                  C.  Make circle smaller and move it around to isolate the problem area further.

                                   

                                  After some trial and error, I settled on the groove on the underside as a problem area.  It even looks bad.  The tangent edges at the bottom of the groove want to intersect at the middle of the part.  Using the steps above, an extruded cut using a small circle (.0001" dia works) that is at least 0.105956" deep will correct the problem.  The circle should intersect the inside tangent line at the bottom of the groove.  This is tricky to achieve, because the garbled display hides the edge as you get near the center of the part.  I selected the tangent edge near a corner of the part and added a midpoint relation to the circle center.

                                   

                                  The depth value of 0.105956" puts the cut just past the depth of the tangent line.  Anything less won't correct the error (actually, the true minimum depth to correct the problem is somewhere between 0.105955 and 0.105956.  I din't feel like exploring beyond 6 decimal places).

                                   

                                  I played around with 'filling in' the cut an found some other strange behavior:

                                   

                                  A.  Roll the model back before the cut and do a Surface-Offset of the groove sides and bottom, using a distance of 0.

                                  B.  Roll the model forward.

                                   

                                  The offset surfaces are no longer anywhere near the groove. In fact, the outer surface is now near the inner surface of the groove.  This is more than a low quality display problem.  These faces and edges are MOVING as a result of adding features to the model.

                                   

                                  Jim S.

                        • Re: hi everybody
                          Christopher Thompson

                          I can see the problem after importing into Pro/Engineer Wildfire 3.0 (export as Parasolid v 16.0 from SW2009), and it is due to some additional surfaces in the model. This explains why the model zoom so far out in the default view in SW. How do you think these additional surfaces got into the model? What CAD software was used to create the origional?

                           

                          After exporting the imported file from Pro-E as a STEP, and importing into SW, a similar image appears with the imported file consisting of surfaces. I have attached the STEP export file created by Pro-E. Perhaps you can repair / delete the extra surfaces in SW from the attached file.

                           

                           

                           

                          Parasolid_import_Pro-E_WF3.JPG

                            • Re: hi everybody
                              scott sides
                              Im not sure what cad software was used to create the model. I did run import diagnostics on the model and it found 2 problems ,I clicked heal all and it fixed them
                                • Re: hi everybody
                                  Anna Wood

                                  Scott,

                                   

                                  If you get a step or iges file from the customer you can open those file types in Windows Notepad.  They are just plain ascii text files.

                                   

                                  At the top of the file in the header section will be what cad system it was exported from.

                                   

                                  Cheers,

                                   

                                  Anna

                                    • Re: hi everybody
                                      scott sides
                                      the file was created in pro/engineer
                                        • Re: hi everybody
                                          Christopher Thompson

                                          Scott,

                                           

                                          If the file is not properly healed / repaired in SW, and you can obtain the original Pro-E file, I can open the file in Pro-E and export as a SW file. The file would need to be Pro-E WF 3.0 or earlier as I can not open Pro-E WF 4.0 or 5.0 files.

                                           

                                          Go to contact information on my website to email me directly if you need help.

                                           

                                          Chris Thompson

                                          www.appianwaytech.com

                                            • Re: hi everybody
                                              scott sides
                                              thanks for the help .I was able to seperate the core and cavity from the part to do the changes they wanted.
                                                • Re: hi everybody

                                                  Hi Scott,

                                                   

                                                  I had a chance to open your model this afternoon and tried something:  I created a coordinate system and exported in IGES (Mastercam tag) and then re-imported it again into SW thinking that a round-trip would give the healer another chance. It does not come back in solid meaning there was a face that wasn't so good when it exported. When re-imported, the Import Diagnostics shows a missing face (as Jim suggests) in one part of the lip/groove detail.

                                                   

                                                  After the roundtrip and then an additional import diagnostics heal of the face, the part seems to check out. I've attached it here. Sounds like you are in good shape now anyway. I just wanted to point out to you and the others on this thread that if you have troubles with imported models, try to "roundtrip" them again by exporting them and them re-importing them. The import healer (for IGES and STEP) is NOT parametric and occurs on import of the file. The import diagnostics is an additional tool when the import healer doesn't catch everything.

                                                   

                                                  Sometimes models are so bad that they need sequential successive repair in order to be healed properly. This is actually something I learned when I was doing ProE back in the day - the same technique can be employed (sequential successive repair) in ProE but without having to reimport the file.