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?
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.
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
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
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.
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.
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.
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.
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
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.