sw lousy dxf file export - my solution

Hi all,
For ages SW outputs dxf files of 2d profiles from a drawing with minute
errors. Most cnc laser or router cam software require flat 2d closed
polylines to cut or machine. SW exports what should be a closed
polyline as a series of lines and arcs with (sometimes) small gaps
between the endpoints. This means you can't use pedit to join them.
If you have express tools you can enter a fuzz factor to heal it, but
it's obviously a work around.
What I do now is this:
In my part file I select the top face of what I want cut. If it's a
split part I select all required faces. Then saveas Acis, select faces
only option and save. You may need to create a 'proper' cartesian
coordinate system, with Z pointing up not out.
Open this sat file in acad with 'acisin', and all the faces appear as
regions. If you arn't familiar with regions they are like a 2d solid.
ie, can't have gaps in the corners because it is a body.
If you explode a region it becomes a sequence or arcs and lines which
can easily be pedited together to a closed polyline.
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I think PEDIT will work if you change the "fuzz distance" setting.
Reply to
Rock Guy
This may save some time and work as well for you. Create a configuration called laser cutting. Open a new sketch and use convert entities to get the profile that you desire. Open another sketch and select the geometry from the first. Use the tools-spline tools-fit spline funtion. Leave it as constrained and give it a reasonable tolerance value ( the default value makes no sense ). At this point I usually crate a simple planer entity from the profile to check it for obvious errors.
On your drawing, create a sheet and insert a view of the cutting configuration. You can then export the sheet as dxf/dwg and it will give you a joined polyline. I suggest R12 version as I've had good luck with it and at this point you should not have any entities in your file that are not supported. I think that the use of the fit spline tool has given the user some control over how splines get exported, but am not sure. Using a planer surface also eliminates the possibility that SW will accidentally export extra geometry ( ie both the top and bottom profiles of an extrude, thus creating duplicate entities, one on top of the other ). Since using this method, I've had no complaints from my laser cutters/engravers. The engraver does not have any fancy software, so I use the same method even with tangent lines/arcs to convert them into continuous polylines. That prevents his laser from reading tangent lines/arcs in the order that they were written into the .dxf file, which rarely makes a good cutting path. Used this method on a Mitsubishi cutting laser, a Trumph, and an Epilog engraving laser, all with no vendor complaints.
This also makes it possible to export ellipses to dxf. Since 2001 ellipses have always exported as the inverse of what they should be, regardless of the fact that its been "fixed" in about 10 different service packs.
Reply to
Interesting reading, I've been using the standard save as DXF for several years with no complaints!
No doubt my sheetmetal vendors are pulling their hair out every time I send them a DXF and haven't bothered to complain.
Thanks for the heads up, if I have problems in the future I will refer to this post.
John Layne
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Reply to
John Layne
Me too... and never a complaint, although I always send DWG.
Reply to
Cam J
fuzz factor is only availbable in 'express tools'. Plus, it's a little irksome to have to actually change the geometry of what should be a closed profile since it was originally drawn closed.
Reply to
Yes, a lot of fabricators strangely just fix the file and never say a word. But the cost will often be in the bill somewhere. Years ago I used to own a cnc pattern shop and I expected bad files requiring lots of fixup. Endless conversations with people on the phone explaining a 'closed' pline etc. I'm really amazed that with it's touted dwg compatability that sw has, ever since 2000 anyways export disconnected loops - with errors- into dxf files. Even a rectangle will usually have one corner where the endpoints are seperated by .00000001" . This is enough for Cam software, especially the cheap stuff that ships with machines to not be able to tell the inside from the outside. Hence my region trick.
Reply to
Howdy Zander -
I lived this one for many years of my life too, but without the high anguish level - perhaps just luckier or different software with higher gap tolerance.
I like your trick. One trick I also use to fix this problem (once in 2d) is a grip edit - Pull the node away and then back again - it healed the micro round off.
This "millionths" round off killed me and also drove me insane. I recall a complicated design DXF'd out of Anvil (A heavy weight you bang things against) and I have to Pline every profile we were wire cutting. Arggg!
Generally, you "endless conversation" statement almost invariable applies to people who have not felt the pain when programming. That's sombody else's problem.
Cool tip.
Reply to
Sean-Michael Adams
I feel your pain, I have the story to end all for acad pline'ing. I machined years ago a 3d map based on gis contours from the government, it was about 10' sq. The data was in dxf format, the file was 30km sq. The gis software only support plines of 500 vertices max so every 500 vertices of these squiggley contour lines there was a break with ---- a gap!!!! Even if you closed the gap the resulting pline chains were so long that back then on a 486 powerhouse it took 15 minutes to complete the join command for 1 pair.
Solution was: I wrote a vb macro that matrixed all the start and endpoints of the plines and found nearest neighbors and fairly intelligently chained them together. If it couldn't solve it it changed the layer and color of the offendors. Net result. 20 hours writing 1 very long and complicated macro and 25mins to process the whole file at the end. I had fun and learned some stuff and prevent carpal tunnel again!
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