Generate sheet metal dxf flat pattern

[ptc-4599805]

Hi,

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).

Thanks,

Adam

[KrisR]

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.

[Bablu]

Please share full details of this process

[JohnMitchell]

Adam,

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

[BrianMartin]

Hi Adam...

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.

Thanks!

-Brian

[ptc-2879375]

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.

Ideas?

Karl

[dschenken]

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.

[DavorGranic]

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.

[ptc-2879375]

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.

Karl

[jzhang-3]

Because we cut block by wire EDM, it will be nice to save cut path as .dxf from model dirctly vs. in drawing.

[ptc-4578749]

Hi all,

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.

Regards

Tomasz

[SolidPerks]

Sorry folks,

I realize this is an old thread, however, still a relevant topic & unanswered. I'll as concise as possible

I have a sheet metal model. I DON'T want to make a drawing file. I want to send a DWG/DXF flat pattern to my cutter.

Can this be exported DIRECTLY from a Creo2.0/3.0 model? None of the above comments lead to believe this is possible.

Thanks!

[spaceghost173]

Still a relevant question. 

Is there a way to export a flat pattern without creating a drawing 1:1 ratio and then saving as a DXF? 

Funny how other software like SW and Inventor figured this out quite some time ago but PTC is over here, wondering what the problem is....

I have 41 sheet metal parts that need to be exported as DXF sheets to send to fab but what I am finding, is that I have to create a drawing file and then save that drawing file as a DXF after I place the flat pattern on that drawing...41 times...hooray.

[pausob]

Not out-of the box.

We ended up making a mapkey and a drawing template.  The template has a single named view set to a named orientation (called "DXF") at 1:1 scale, and without format or border, etc...

The mapkey 1st saves the model's current view as "DXF" and then creates a new drawing using the template, then exports it...

So you point the camera down on the flat pattern, then activate the mapkey, which is bound to a button on the toolbar, so it's a 2-click operation, thought it would get tedious for 41 parts.

[Bablu]

go to file and options than configuration editor
After clink on configuration editor you see the find options below it click
on it.
New pop up tab will be open then type in key word dxf_out and enter after
completing this you can see the dxf_out drawing scale click on it you see
its valve is no change it into yes and click on add change then ok
Now your dxf file is 1.1

[ABMartins]

I was able to create a mapkey similar to the one you mentioned... but I am still wondering if we can export DWG directly from 3D model flat pattern.

Is it possible nowadays?

[StephenW]

@ABMartins 

File, Save-As, change the file type to DWG.

[tbraxton]

@StephenW  is it now possible to save a 2D-DXF file from part mode? That is the query from @ABMartins above as I read it. He is looking to avoid having to create a drawing to export the DXF.

[StephenW]

@tbraxton

 I am on creo 6. I can save as DXF or DWG directly from a model using file - save as. In Autocad, it appears to me as a tesselated model. I am not an autocad user so I am not familiar with import options. It may be of value to someone who understand how to manipulate autocad data better than me.

If I was doing it, I would export via a drawing to guarantee a 2d export for a flat pattern.

[ABMartins]

I tried this but output file has several triangulated lines as you can see below:

I've done some research but I don't know why this happens and how to avoid it. I want to output just boundary solid lines of the part.

[ABMartins]

I've found this article: https://www.ptc.com/en/support/article/CS341495

So if I'm not mistaken, currently it is not possible to export a flat pattern directly from 3D model without these additional triangulated lines.

[kdirth]

The DXF of a model is, by definition, a triangulated model.  Creating a DWG is the same.  Part of the problem is the limitations of AutoCad when dealing with neutral files.

A short lesson on the origin of DXF file format from the wikipedia: "DXF was introduced in December 1982 as part of AutoCAD 1.0, and was intended to provide an exact representation of the data in the AutoCAD native file format, DWG (Drawing)."