Creating DXF's directly from CAD Models

[kramarao]

We are seriously looking in to 3D Annotations(Model based Definitions) on the 3D cad models, specially parts. Having gone a fair way in setting up the templates with what ever available in Pro/E Wildfire 5.0 (M200), realised that DXF profile generation on Sheetmetal Developed views are not possible in the part mode. That functionality is only available in the drawing. After contacting PTC support and getting a "NO" answer, ended up doing a mapkey to automatically create a temporary drawing, generate the DXF profile and erase the drawing from session.

Just wondering whether others are also having similar issues and how they are getting around the issue?

Cheers

Kashyap

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[JOHNQ]

DXF (Drawing Interchange Format, or Drawing Exchange Format) is a CAD data file format developed by Autodesk for enabling data interoperability between AutoCAD and other programs.

DXF in the CAD world is just a drawing to other programs. It was like developed in 1980's by AutoCad just for transfer drawings of autocad to other Cad programs.

Sounds like you want to exchange an Actual Model which is impossible. I am wondering what exactly your looking for as a end result.

John

[dschenken]

DXF Supports 3D entities. Search for "DXF Reference - Autodesk" The version I've found is for AutoCAD 2008.

[BrianMartin · Accepted solution]

Hi Kashyap...

I believe most users would surmise that to extract a 2D format file (like DXF) from Pro/ENGINEER, you'll have to create a drawing. This seems reasonable given that Pro/ENGINEER is a 3D modeling package and you're forcing it to collapse all of that information down into a 2D view for a DXF. So... I don't think this points to a lack of functionality in Pro/ENGINEER. Of course, this doesn't solve your problem... you still need that file for your fabrication team.

Under the circumstances, if you've managed to create a mapkey to generate the required view, export it, and erase the temporary drawing, I think you've found a great solution. Take that mapkey and make a nice custom icon for it. Apply the mapkey and icon... and drag the mapkey into your screen menus. In this way, everyone can "print" a quick DXF just by clicking an icon on the desktop. The icon simply runs your mapkey.

I think this is a really nice solution and I wouldn't necessarily waste any time trying to find something "better". You could write a J-Link or Toolkit application... but why? Your mapkey already does the same thing and it works without spending any additional money to develop another solution.

As a side note... I tried a different method of creating a DXF before I wrote this response. I went into Creo View 1.0 (which will read all Wildfire 5 models). I added a cross-section and turned on the "2D" option. I was able to save the 2D cross section as a DXF without even having to launch Pro/ENGINEER at all.

For a completely FLAT sheet metal model, you could totally use Creo View to create your DXF without ever creating a temp drawing and without requiring a mapkey.

Still, I think your best option is to stick with what you have. Creo View did a nice job... but why enter Creo View just to make your DXF when you already have it working native from Pro/E?

Good job with the mapkey... and good luck! I think you answered your own question!

Regards,

-Brian

[kramarao]

Very Useful info.

I will give it a try in Creo 1.0 when I get our licenses updated !

Thanks

Kashyap

[BrianMartin]

Hi Kashyap...

I was actually talking about Creo VIEW 1.0, not regular "Creo 1.0" (also known as Creo Parametric 1.0).

Creo VIEW can be used now... even before you upgrade to Creo Parametric. Because Creo View can read all legacy Pro/ENGINEER files, you can try it out now without having to upgrade the rest of your system. Of course, licensing for Creo View is separate from the rest of Creo. A standard license does cost additional over and above your Creo Parametric license. There's a free version of Creo View (called Creo View Express)that you can download and try. It probably doesn't have the DXF output option, though.

Thanks...

-Brian

[kramarao]

I tested it on Productview 9.1 client. What you have said has worked.

Many thanks again.

At some stage(time permits), Could you please also have a look on my other question about

Balloons on 3D assembly models (Again related to annotating models), currently cannot show BOM's/Balloons directly on models.

Regards

Kash

[kramarao]

Also the above dxf from Product Vew/Creo View is olny available in Creoview Client.

Its not available in free versions of Product/Creo View

[BrianMartin]

I assumed that would be the case... export functions like DXF are reserved for standard licensed copies of the software (not the free version).

I'm thinking about your problem and trying to come up with other approaches. I'm not sure there's a better way but maybe there's something else we're overlooking.

I will definitely go back and take a look at your other question, too. I was away from the message board for about 6 weeks and I missed several questions. I'll go look for it now.

Thanks!

-Brian

[bridgel]

I am trying to do a similar thing. I have a rigid/flex circuit board modeld. The flexes are done in sheetmetal. I want the outline of the entire thing as a DXF so I can bring that in as my board outline in Mentor Graphics. I cannot find a way to export this. I always get the lines between each board and flex. Any thoughts?

[KevinBradberry]

I'm probably confused because I'm sheetmetal illiterate, but I don't understand the goal here. You want to create 3D Annotations so why are you worried about exporting DXF. How will that help you create the annotations that you desire?

[kramarao]

Hi Kevin,

Idea of 3D annotating the models------ are to save 2D drawings, there by saving cost to the company in creating/managing additional models

Idea of exporting DXF is to convey outer profile information of the sheet parts for the LASER to cut. Presently DXF can go only from drawings, not directly from models. If we have to do drawings to service this, then the original intent of 3D annotating to save the process defeats.

Kash

[KevinBradberry]

Hey Kashyap,

I understand the logic, now. Thanks for that.

[jzhang-3]

We have the same issues for wire EDM cuting. I hide solid model and save curves as .dxf in Creo 2.0, it shown nothing when I open it again. Have you find a way to save curves from model to .dxf dirctly?

Thanks,