flat patterns as closed poly-lines?

Hi,
I have a lot of flat patterns to export for laser cutting. I'd like
to be able to do 2 things:
1: Have the profile be a closed polyline instead of multiple
disconnected line segments.
2: Eliminate the bend lines (secondary)
Any ideas for this?
Thanks,
Zander
Reply to
Zander
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Possible solution to #1. Save the SW flat pattern drawing as a dwg file. Open the dwg file in AutoCAD or DWG Editor and use the PEDIT command to join all the lines into a polyline.
Type PEDIT into the command line and hit enter. Choose "m" for multiple and window select all the lines, hit enter. Say "yes" when asked to convert to polylines. Choose teh "j" option to join the lines and hit enter. You should now have a closed polyline region.
Rob
Reply to
robrrodriguez
Hi Rob,
Yep, I'm very familiar with pedit et al. But a streamlined work flow for hundreds of flat patterns for both me and the fabricator requires that sw saves out a closed polyline, which it's never done afaik. They added a 'merge endpoints' option recently but it appears to have no effect. Another way is to select the face of the flat pattern in part mode, saveas acis and choose 'selected face'. This will save out a region which can then be exploded in acad. But ideally the job of exporting the dxf files would be done by 'task scheduler' from the drawings.
Zander
Reply to
Zander
Zander,
Forget about using other apps, the functionality is already there. I do at least a dozen flats per week with SoiledWorks since 98+. Here is the answer:
In the sheet metal part: 1) Right click on Flat Pattern feature in the feature tree and select Edit Feature 2) Select Merge Faces option Perform these same steps on your sheet metal part template. This will provide continuous lines.
To remove bend lines in the sldddwg flat pattern:
In the feature tree, traverse to the drawing view and expand the part features. Expand the Flat Pattern feature, right click the Bend Lines feature and select HIDE.
Regards,
Dave Herbert
Reply to
Dave
Hi Dave,
That's excellent! Thanks! When you mentioned 'merge faces' it reminded me that I havn't looked at that option for about 5 years and totally forgotton about it - plus I never knew that it would produce closed pline export data.
Thanks again,
Zander
Reply to
Zander
Good tip Dave and good discussion. I do this everyday for our fab shop, but we do not need to have the laser profile dxf file as a polyline. I'm curious why your laser software requires this. I suspect that doing this might force you to eliminate any extraneous short segments - anything shorter than the beam offset causes a program error. We always send the layout as lines and arcs. The only other thing we do is for ellipses, turn pellipse on, this turns the ellipse into short segments that the laser program handles (this involves redrawing the ellipse). BTW, we use NCell and NC Express for our Mits lasers and Finn-Power laser, and sometime Fabriwin for hand-coding.
One way to quickly eliminate the bendlines and bendnotes is turn off sketches on the drawing template and then right click the flat view, click properties and turn off display sheet metal bend notes. I do this before adding any other notes or dim's to the drawing view. Then use edit, copy to DWGeditor to put the view into dwgeditor. I stopped using Autocad for transferring patterns last year and find dwg faster. Some parts of this can be automated with a macro, and perhaps someone with programming skills could automate the whole process.
Diego
Reply to
Diego
Good tip, thanks.
One problem we have here is that we don't usually produce our sheet metal parts using the sheet metal feature but rather we turn our solids into sheet metal parts and in that case the merge faces option is not available. In parts that end up having splined edges we typically have to go into the exported dwg and manually clean it up by tracing over thee splined edge with a p-line. We don't use the sheet metal feature because most of our parts simply cannot be created using the functioality of sheetmetal in SW.
This works fine if you have to do it every once in a while but if you have lots to do I don't know of any other method but the brute force way.
Steve R
Reply to
Steve Reinisch
I'm curious - what is it in your parts that they end up as sheet metal parts, but yet you can't use the sheet metal tools to produce them? Do you do a lot of in-context stuff to define the geometry? Start with imported sketches?
WT
Reply to
Wayne Tiffany
We do a lot of aerospace type parts that have wierd curves and conical shapes. We also find that doing cones using the sheet metal features does not result in a true conical shape, and if we end up with a truncated cone the splined curve usually requires clean-up so our laser guy can use it.
Steve R
Reply to
Steve Reinisch
Another way to eliminate the bend lines is to right click on them in the drawing view and select hide.
Best, Marty
Reply to
Marty SLC
how do you save them as polylines? when i do a save as DXF i just get the individual lines. in SW2007, Pedit doesn't even work on these.
Reply to
Hunter

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