9 Replies Latest reply on Aug 15, 2014 8:40 AM by Dakota Baird

    Importing IGS and converting to solid

    Dakota Baird

      I am receiving an IGES/IGS file from a customer using Tekla. They export as an xml in their Tekla software and convert it to an IGES/IGS file. When I import this assembly into Solidworks I am using the options in import dialog box for IGES/IGS to try and create solids. We have also tried doing .dxf as well and even importing their native .ifc files. Attached is also a summary of our issues we are running into. Basically if we import the IGES/IGS file we get the cut information on the tubes but they are surfaces and not round tubes. If we import the .ifc Tekla file we get the round tubes and assembly but not the cut information for the tubes. Has anyone come across this issue/know of a solution. Of course modeling these based on the geometry will work but because of the size of the assembly(entire hand rail structure with multiple floors) it would take days to reverse engineer these parts. Any advice or help is much appreciated. For those wondering our company has an add on for Solidworks that generates cut information for the parts that is read by the 3D cutting machine so we need both the geometry of the tube as a single part and the cut information to process them.

       

      Thank you

        • Re: Importing IGS and converting to solid
          Evan Dlugopolski

          What exactly do you mean when you say cut information? 

            • Re: Importing IGS and converting to solid
              Dakota Baird

              If you take a look at the word document attached you can see in the first picture it doesn't pick up the cut features on the tubes. Those intersections should be cut to fit together. If you import the .ifc format you get the smooth tube but the end cuts and intersection cuts are not present. This is something they model in their Tekla software that is not being translated either by the export from Tekla or the import to Solidworks. But if you check the IGES/IGS file you can see those cuts are present and the geometry of those cuts are present but the tube geometry is not a round tube it is a faceted.

               

              Edit: Sorry you might be referring to when I said my company's addon generates cut information. If that was the case then I mean NC code that is read by the 3D cutting machines. We generate that based on the geometry of the parts and need a solid body to do so.

            • Re: Importing IGS and converting to solid
              Jamil Snead

              I'm guess the issue with the IGS having faceted tubes probably results from wither the xml export or the conversion between xml and igs. I would check export settings in Tekla and see if there is some setting that converts arcs to line segments or something. I don't know anything about xml format but maybe that file type by nature can't process arcs, similar to STL. So I'd try exporting to some other format from Tekla. Also, what software are they using to convert xml to igs?

                • Re: Importing IGS and converting to solid
                  Dakota Baird

                  Ok I contacted Telka support and they explained the bigger issue here. Basically Tekla models their cuts on the parts using anti-matter material and Solidworks does theirs by creating a void but uses a different logic. That information is in the .ifc file from Tekla BUT because the process logic is different Solidworks can not read that information. So I have two possible solutions but I am not sure whether either is doable. The first solution is to figure out how to do a 3D trim in assembly mode within Solidworks for the .ifc file because that at least has the proper tube geometry other than the trim cuts. The other is to use the IGES/IGS file and somehow have Solidworks create a solid part using the many surfaces that make up the tube. Right now I am not sure how to do either. Even if I tell Solidworks to create a solid part using the IGES file it does not. The Tekla support tech informed me that they can export to just about any general file format including the following: DWG, DXF, SDNF, SDNF(PDMS), PDF, PDMS, PDS, XML, DSTV, IFC, STP, STEP, IGES, EXCEL, WORD, Comma delimited, SKP, SACS, FEM, PML, HLI, SCIA, Calma, DGN

                   

                  Our customer tried doing this directly and we get the same results as we did before. So if anyone knows how to do this within the assembly mode that is what I think is the best solution. To do it on the part level would be doable but would require days of work for a single assembly and this customer has hundreds of assemblies.

                    • Re: Importing IGS and converting to solid
                      Jamil Snead

                      For the tubes that are cut completely by the side of another tube (for example a T connection), it is fairly easy to do from within the assembly. Edit the part that needs to be trimmed in context of the assembly, then use the Cavity tool. In the Design Components field select the tubes used to trim and click ok, then when the Bodies to Keep dialog pops up choose "Selected Bodies" and just keep the main tube body (will probably be body 1). That's it, you can then exit the part and proceed with the next tube.

                       

                      However for the joints where both tubes need to be cut, for example the corners where each tube gets a 45 degree cut, that is not so simple. You might need to establish a plane in the assembly where you want to cut the tubes (may require sketching), and then use that plane to split each part.

                        • Re: Importing IGS and converting to solid
                          Jamil Snead

                          So here is one method to do the corners. Edit one of the parts in context of the assembly. Then start a 3D sketch and do an Intersection curve using the outside surfaces of both tubes as the selections. This give you two ellipses, and delete the one that isn't along the cut. Next use that sketch to make a fill surface (which will be the cutting plane), and use that surface to do a split feature. Pick the option to consume cut surfaces and select the scrap piece to consume. Once one tube is cut like that you can use the old cavity feature on the other tube.

                            • Re: Importing IGS and converting to solid
                              Dakota Baird

                              Thanks for your time. I was able to trim corners using the 3D Sketch of the intersection and then extrude cut that sketch. The cavity was not working on the assembly most likely due to the import issue. I am going to test different export methods from Tekla Structures to see if they generate a better import into Solidworks. I even tried to macro the corner process and apply to the other corners but because of the import issue it did not work either.

                                • Re: Importing IGS and converting to solid
                                  Jerry Steiger

                                  Dakota,

                                   

                                  Try the STEP output from Tekla. The preferred file types to import into SolidWorks are Parasolid, STEP, and IGES, usually in that order. Parasolid is the best because it is the native file type for SolidWorks, but you don't get that choice from Tekla.

                                   

                                  When it comes to importing files, it shouldn't matter how Tekla or SolidWorks handle geometry; you are dealing with a neutral format (Parasolid, STEP or IGES). You may need to work with people supplying the neutral format files to find the best options for each file type. You also need to make sure that you have your options set in the best way on the import, but it sounds like you have already spent some time on that.

                                   

                                  Jerry S.

                                    • Re: Importing IGS and converting to solid
                                      Dakota Baird

                                      Thank you for the suggestion. I asked Tekla Support for the types of file they can Export and STEP is on the list so I will have them try that. I even pulled the .igs file I received into Rhinoceros to see if I could clean up the edges and smooth them out. Turns out a lot of the edges were not closed/missing when I imported it into that software so it could be an issue with the export and have nothing to do with Solidworks importing.