Guest ldobson Posted June 8, 2010 Share Posted June 8, 2010 Has anyone else had problems creating a dxf file for CNC cutting machines with unfolded sheetmetal parts that have holes from the "cut sheetmetal part" command that leave inside and outside surface lines that confuse the cutting machine? How to remove these redundant lines so the cutting operation can work? Quote Link to comment Share on other sites More sharing options...
Cary OConnor Posted June 8, 2010 Share Posted June 8, 2010 Try to make sure your part is parasolid. ACIS sometimes creates duplcate lines in the 2D export. Cary Quote Link to comment Share on other sites More sharing options...
dberge Posted June 9, 2010 Share Posted June 9, 2010 this happenes when the cutting part is not straight on the sheetmetalpart. I remove them in autocad...... too bad the `modify affected bend` tool is buggy and limited, that should be the alternative Quote Link to comment Share on other sites More sharing options...
Cary OConnor Posted June 9, 2010 Share Posted June 9, 2010 too bad the `modify affected bend` tool is buggy and limited, that should be the alternative Could you clarify that statement so I understand the issue. Thanks Cary Quote Link to comment Share on other sites More sharing options...
dberge Posted June 10, 2010 Share Posted June 10, 2010 Hi Cary the `modify effected bend` with a `custom profile` cut-out is limited to 2 bends or 1 bend with stock. Using more gives a currupted unfold. Also the results of the modify-effected bend are not shown many times in 3D or give errors. i attached a sample if this would work , it would be a great tool for me. regards Wim Scene2.ics Quote Link to comment Share on other sites More sharing options...
Cary OConnor Posted June 10, 2010 Share Posted June 10, 2010 I'll send that case to R&D to take a look at. It is probably a mapping issue from 2D to 3D (how it calculates what it looks like in 3D). Cary Quote Link to comment Share on other sites More sharing options...
Guest ldobson Posted June 10, 2010 Share Posted June 10, 2010 Try to make sure your part is parasolid. ACIS sometimes creates duplcate lines in the 2D export. Cary 28897[/snapback] I changed from ACIS to Parasolid & redid the unfolded drawing ~ still didn't work. They have been redrawing in their software to make it work. Can't we produce an overlap-free drawing for laser-cutting? Let us pick which side of the sheetmetal to project. That is essential in my work. Larry Quote Link to comment Share on other sites More sharing options...
Cary OConnor Posted June 10, 2010 Share Posted June 10, 2010 Larry, Please send the files so we can review the issue. Cary Quote Link to comment Share on other sites More sharing options...
dhovatter Posted June 11, 2010 Share Posted June 11, 2010 I do not know what CNC program you use but I use Master Cam. I orient my part with tri-ball getting it correct relationship to machine and where 0 should be then export as a parasolid (.X_T). Then bring it into Master CAM. Dallas Quote Link to comment Share on other sites More sharing options...
Mats Andersson Posted June 11, 2010 Share Posted June 11, 2010 I use ironcad to get 2d geometry for my wire edm. I always make a 2d curve and export that via caxa draft as a dxf file that I can send to the machine. If I have problems with duplicate lines or other things it always is my own fault. If I do it correct I never have problems doing it this way. Quote Link to comment Share on other sites More sharing options...
anilsson Posted June 23, 2010 Share Posted June 23, 2010 I use ironcad to get 2d geometry for my wire edm. I always make a 2d curve and export that via caxa draft as a dxf file that I can send to the machine. If I have problems with duplicate lines or other things it always is my own fault. If I do it correct I never have problems doing it this way. 28920[/snapback] I want to export dxf geometry for laser-cutting from the 3d scene, no work around Quote Link to comment Share on other sites More sharing options...
cborer Posted June 24, 2010 Share Posted June 24, 2010 (edited) I want to export dxf geometry for laser-cutting from the 3d scene, no work around 29026[/snapback] Well of course that does not work as it is 3d, ....but in the scene it would be nice to export 2d dxf from the cross section of a shape (like we already can import to a cross section). Which is an old ER of mine. Carlo Edited June 24, 2010 by cborer Quote Link to comment Share on other sites More sharing options...
anilsson Posted June 24, 2010 Share Posted June 24, 2010 Well of course that does not work as it is 3d, ....but in the scene it would be nice to export 2d dxf from the cross section of a shape (like we already can import to a cross section). Which is an old ER of mine. Carlo 29037[/snapback] what I mean is, choose an surface of one part and right-click and select export dxf or select a unfold sheetmetal part and make the dxf-export, then the software make an overlap-free drawing perpendicular to the surface, faster than to move between different applications. I think Solid-Edge has this possibillity Quote Link to comment Share on other sites More sharing options...
Cary OConnor Posted June 24, 2010 Share Posted June 24, 2010 Does your CNC machines support IGES? If so, you can create the surface as described above and export to IGES. Cary Quote Link to comment Share on other sites More sharing options...
cborer Posted June 25, 2010 Share Posted June 25, 2010 Laser always want dxf! Quote Link to comment Share on other sites More sharing options...
dhovatter Posted June 25, 2010 Share Posted June 25, 2010 question: are you exporting from Scene or Drawing. I do not do much with sheet metal I but did a test with unfolded part that I created. I created in SCENE and unfolded. Opened blank Drawing and then scaled it up to 1:1. Did export sheet to .dxf. I had to select force true Representation box and export drawing view, and force 1:1 I had to use force True Representation (slower precise) because the arcs came out as vectors if I did not. Then I tried opening it in True View and it came in fine. Dallas Quote Link to comment Share on other sites More sharing options...
Cary OConnor Posted June 25, 2010 Share Posted June 25, 2010 Hi Dallas, I think the issue is the Cut Operations performed in 3D. When you unfold the sheet metal, the cuts will not necessarily be straight since they are mapped from a 3D down to the flat. Which is correct. However, this can cause the issues posted. One way to resolve it is to just select the top or bottom surface of the unfold and create a surface. From there you can create a drawing of the surface to resolve the issue. What is requested is the ability to skip the drawing and just export the surface. We have had this request before (as Carlo stated). R&D will have to look at the feasibility for this. Cary Quote Link to comment Share on other sites More sharing options...
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