9 Replies Latest reply on Feb 12, 2014 7:54 AM by Kevin Sizemore

    Imported Part Editing

    Kevin Sizemore

      I have an imported part from a 3D scanner that has hand sanding on it so there are some imperfections I want to fix and there isn't a straight surface to work from. Can't use feature recognition either. Most of the part looks like this, many facets and no real radii. Is there a way to "pull" material up? I have tried move surface and haven't been successful. Maybe knit a surface around the opening and somehow fill it in? The hatched area is the are I want to fill in.

      image.jpg

        • Re: Imported Part Editing
          Jeremy Feist

          if you are on 2013 or newer, you could make the surfacs to close in the area you want filled and then use the intersect feature fill it in.

           

          earlier versions you eil need to either delete faces and construct new ones to knit into a solid, or fill in the area with a solid and use the combine feature.

           

          or and replace face mght be helfull in some areas.

            • Re: Imported Part Editing
              Kevin Sizemore

              I am in 2013. I will look into the intersect feature but how would I go about making a surface that would cover the opening?

                • Re: Imported Part Editing
                  Jerry Steiger

                  Kevin,

                   

                  You might be able to Offset Surfaces, with offset=0, of the surfaces to the left and right, then use Untrim or Extend so that they run over the hole, then Trim and Blend to match the blend in the center. At that point you can delete the two original surfaces and then Knit the surfaces together to get back to a solid. If it were only that easy!

                   

                  Jerry S.

                    • Re: Imported Part Editing
                      Kevin Sizemore

                      Jerry,

                       

                      Thanks for the help. I have been able to take your advise and overlap the faces using untrim (nice feature) and then using trim to eliminate the extra surfaces. I am a greenhorn when it comes to surface work on a dumb model. I wish there was a way to only stretch or pull a surface in one direction. I was having to using a percentage overage with untrim on the entire surface and do a lot of trimming.

                       

                      Ultimately, I need to get three skins out of the file that I need to thicken to .070" to represent the final part. I do this by inserting an empty part, edit the part, zero surface offset from the original part and then use thicken. I am having trouble getting some of the faces to thicken to .070" because the offset is too much. I get the "cannot because zero thickness" error from Solidworks. I have tried to work around the faces that will not offset and use fillet from the surface menu to get a blend but not having great success with that either. Usually, the problem faces are all terminating at a central point. I have also tried to shell the part but getting the same error. Is there a way I can merge multiple faces together as a blend so that the offset would not be constrained by a smaller face?

                       

                      Kevin

                        • Re: Imported Part Editing
                          Jerry Steiger

                          Kevin,

                           

                          You can use the radius of curvature display to see where the problem areas are. You can run your cursor over the part when it is in that display mode to get values for specific points. If you are having problems where several faces come together, you might try trimming out a circular or elliptical opening around the meeting point and then use a Fill Surface to close the hole.

                           

                          Jerry S.

                            • Re: Imported Part Editing
                              Kevin Sizemore

                              Jerry,

                               

                              Your advise has been invaluable. I have used just about everything you have suggested to get what I need. I feel much more comfortable working with "dumb model" surfaces now. I was able to delete and fix many offset problem areas on the part with the delete & fix or delete & fill command, as well as using untrim to overlap and create missing surfaces. I have yet to try to shell the part but I plan on turning on the curvature display like you suggest to see the values and fix problem areas before I actually get an error.

                               

                              Kevin

                              • Re: Imported Part Editing
                                Kevin Sizemore

                                Jerry,

                                 

                                Hopeful on the last response, now stuck again. I am working with a model that does not want to cooperate.

                                 

                                Careful not to distort the part and fixing (delete & fill) only areas that appeared to be the worse (several faces ending in a single point) I have only increased the minimum radius of the curvature from the original 0.001" to about 0.006". The next MRofC distorts the part. And that is 70 some deletes later. Not sure I am looking at this problem correctly....

                                 

                                Even trying to delete the surface and using fill surface seems to be imperfect even resulting in peaks or valleys in the mesh.

                                 

                                Do you know of a service that would be able to work with the model to get the desired result. In my case, I need the minimum radius to be no less than maybe 0.075" without distorting the model.

                                 

                                For background, I need to shell the part for the purpose of mimicking the product. The product is a layer composite that is 0.070" initially, 0.050" finished. It would most likely be at least three different parts that are combined after the mold or form process.

                                 

                                Kevin