I would like to know what is the shortest way to generate sheet metal dxf flat pattern. Now, i'm using drawing part with empty template and set 1:1 scale. Is it possible to make dxf flat pattern clicking on 3d model? I use this method on the other soft ( SW, UX).
What we do is create the flat pattern in the model, suppress it, then create a family table with the generic and the flat pattern as an instance.
Once this is complete, in your drawing, do an "Add Model" and choose the flat pattern instance, and you will be able to place the flat pattern.
If you need more details, please let me know.
In Creo 1, to create the 3d flat pattern - go to File, Prepare, Model Properties. Under Shett Metal, change the Flat State Instances and create a family table flat pattern tied to the shett metal part.
In WF5 this was under Edit , Setup.
For Creo 2, it will be in the floating tool bar at the top of the modeling view.
Once created it can be put in any drawing at full scale then save as DXF
What John says will work. But Kris' technique is also valid. The Flat State function is somewhat different that Kris' technique. Both will create a flat pattern. Once the flat pattern is created, both techniques rely on you to export the drawing to DXF format.
I suspect you're sending the DXF to a waterjet, flame cutter, or other sheet metal cutting device? If so, you may want to pay attention to the bend allowances, too.
Thought I'd see if anyone has any more comments on this. All of the existing responses seem to miss the OPs actual question. Assuming you have already generated a flat instance (and we show it on our drawing), how do you generate the final DXF file that gets sent to manufacturing? We currently do it the way that the OP does. Create a new drawing, scale 1:1 and save as DXF. Would prefer a way to do it directly from the part file, or better yet, from the assembly that the part is used in.
He asked two questions.
1) What's fastest way to get a DXF of a flattened sheetmetal part?
2) Can it be done from the model?
The first answer seems to be, create a flat state and then place a view of it on a drawing.
The second isn't answered, likely because there is presently no way to do so directly from the model.
I suppose using a CNC module could send data directly to manufacturing without a DXF at all.
Fastest is to give manufacturing their own seat of Pro/E or Creo or whatever the next market spin is.
Maybe slightly faster way than exporting from drawing is making Xsection of flatstate part, then opening it in Layout and then export to dxf.
You skip few clicks and lose also bend lines that you dont need when passing dxf for cuting.
Tho something like icon for exporting conture of flatstate(in flatstate preview window) to DXF would be nice improvement to Creo.
We actually put bend lines on our DXFs because we laser etch them at the same time that we do the cutting. But I'll have to look in to that because I don't know anythin about the Layout functionality.
Because we cut block by wire EDM, it will be nice to save cut path as .dxf from model dirctly vs. in drawing.
two things which are helpful:
PDM with cad worker
and a drawing template with three sheets (bent part, measured flat pattern and flat in 1:1 scale)
with that creating a drawing is quite quick (nearly automatic)
after checkin to PDM cad worker will execute creation of PDF and DXF file. The next is to create a subprogram to collect those files from system.