yepp.....ran into this problem in the beginning and got a few unusable parts from the laser cutting company. After that I always create a new view, wich I am sure is right and then name it "flat pattern view", or use the "insert flat pattern view" option in the drawing mode. Krister
Bob Draper skrev i diskussionsgruppsmeddelandet: firstname.lastname@example.org ...
Just finished creating a couple hundred sheetmetal dxf's individually,
> from flatpattern views on a blank 1:1 drawing template, and found the
> dxf's created are not truely flat but slightly askew.
> When I return to the part's flatpattern config at a front-view the
> part appears flat. However if I then select the flat-face and a
> normal-to view the part bucks up a couple of degrees to a true flat.
> This became my workaround, select normal-to flat face then drag
> current-view to dxf template.
> Normally I would then bring these dxf's into Merrymech's cadkey
> converter without problem, then tool and generate nc code over to a
> turret punch. This time around I ran the dxf's into our optimation
> laser nesting software where the problem was noticed, as the
> optimation puked trying to put a zillion tabs around the cut path. >
> So Im not sure how long this has been happening or if I inadvertantly
> changed a setting.
> Im currently using swx2003 sp3 and sp4, but have recently loaded 2004
> beta and pre-release.
> Most of my bttm up parts have many configs and holes cut in context of > an assembly.
> I also use an isoview macro in assemblies.
> Anybody else have this problem?
> Bob Draper
Any idea what causes this? Could it be extruding the base flange in the wrong direction?
Now that I can't trust flat-pattern to be flat. it'll be a big hassle to create a new view each time around with hundreds of dxf's to produce. Be nice if someone was able to make a macro which would; upon selecting a face, 1. flatten the part, 2. create a derived config called Flat 3. and create a normal-to-that-surface view
Even better would be to then; 4. open a 1:1 template called Dxf 5. insert that view onto the drawing 6. save as dxf in same folder as part with parts name.
That's a good tip for creating sm-flat-pattern config. Up to now I've been opening up a drawing template and selecting flat-pattern from a named-view option to get the flat child.
But the problem I was trying to get across is that my dxfs are indeed created from a derived "true" sm-flat-pattern view, yet are not deciphered as flat in Optimation software. When I open the part, select the derived sm flat pattern config, and a front view, it appears flat . If I then select the true flat face and then select normal to view, the part appears to moves slightly towards me. I.ll mess with the base flange sketch planes and drw-dxf template , maybe that'll help
PS Just noticed Amada has a solidworks add-in "Sheetworks", ap100 interface, ever messed with it?
No, I'm just using the models front view to look at the derived child flatpattern view, which was created from parent when insertng into a drawing. I thought that when I go to that child flatconfig and select a front view which the original sketch was created in, it would be the same 2d as the drawing flatview. But when I highlight the face of the flatpattern and select normal-to-view it moves slightly.....almost as if my world view is off a bit, story of my life ,... this is giving me a headache.
Makes sense,you may have identified the problem it here
Wow,now thats powerful stuff! People like you and Guy Edkins and Dom "Flipper" inspire me to endeaver to learn more than just using the software!
So I assume the external boundary can't be broken up and must have tabs added to it?
You know I ran into this very problem, tonight at work. The CEO asked me to model(with solidworks) a golf divot/spike tool from 14ga SS with our logo etched on it. He wanted 300 for important CEO stuff. (its good to be king) So I created two dxfs , 1 with complete internal logo and outer boundary, the other just the external boundary. I then generated 2 identical nests of 14 in a row, fron the 2 dxf's. ( our 2000 watt amada has a 125kb filesize limit) Edited the GLA file in the first nest, replacing all the cutting conditions to e10 etch, and had the laser operator run the etch nest first, than overlay the cut nest after to produce the parts. Well I had to add a couple tabs (microjoints) as they popped up over the rollers and wasn't able to use the trap door, as usual. Anyway the CEO rejected the parts because of the brown marring from the initial cut. So I added a leadin cut, but with our Opti software the leadin disappears when using tabs. Apparently we gave that option up for under the clamp and common line cutting. Optimation is limited in that regard. And our laser operators cant dial in the conditions on thicker stainless to allow a pierce cut, 16ga max. So I tried breaking up the boundary of the "cut" dxf into an open contour that would create microjoints as you spoke of with internal cutouts. Theoretically I would still have my leadin and tabs. Rejected! The only solution left was to run the etch nest, then run the cut nest with leadins but no tabs, forcing the operator to stop the laser each time 1 part was cut thru.
Are you able to manipulate leadins, pierces and cutting conditions with your app, or do you leave that to the laser operator? Or perhaps your product doesn't require a variety of settings.?
Ahhh, sounds like your unfolding software is like API/Amada... wants to grab and unfold directly from the model, and not from a 2d drawing. Hell, Amada wont even unfold the part if it has the Flat pattern FEATURE .. (it needs to have Insert bends/Process bends)
I got sick of the crap I was getting ( as well as sometimes losing the orthagonal flat orientations). I dump the flat pattern to a drawing doc, parse the geometry right from the drawing view, and write to whatever file format is needed.
Again, Amada/API will just 'disappear' from the screen (crash) if everything isnt right with the outside boundary. Thing is, in Amada laser (but not Punch)you HAVE to break up the geometry into peices to do any type of repositioning cuts, so you just have to hurry up and write the NC code, and then NOT save your work. (Redo the same work every time for every part!)
sigh,,, I'm still doing much the same.. Im suprised none of these CAM apps has a "Government Work" module that will let you take off the training wheels in instances like this. Im slowly working in my own NC Code generator, at least for the Laser. I'll probably end up nesting and toolpathing flat patterns directly from a SW drawing, possibly using blocks tied to dxf files, if the flat patterns dog the app down too much.
I used to write 4-5 axis CAM apps (machining centers/Mill), and the thought of these companies charging four figures, for a single tool, and only 2 axes, and not being able to do it correctly, well, ..... err, dont get me going. ;)
I gave up on trying to post clean code and now have my own "post" that takes OUT the crap (like trying to put in a .100" leadin cut for a .025 diameter hole) and puts IN the crap they missed (like changing the Gas settings for engraving, etc, while the tool is positioning, and NOT on the way down; or removing the redundant cuts myself, because the common-line cutting is so fragile: they apparently tied the common cutting to the GEOMETRY, and not the TOOLPATH. If it senses any probs in the Geometry, the Toolpath fails.
As far as microjoints go, I put in a bare minimum on the part (again, Microjoints were tied to the damn geometry, and not the toolpath: Microjoints are just places where you DONT CUT. Ive never recieved a model from a customer that required a microjoint FEATURE)
I wrote a 9000-series NC-Control macro that hooks G01, and automatically replace the G01 cuts with my own macro calls .. the NC macro allows the operators to specify how wide, and how far apart it should "add" a skip in the cuts. Comes in handy when the part starts warping, ie, every 12 inches, add a .030 "microjoint", etc,etc.