Sheet metal

[as-2]

Hi,

How to export flat pattern of sheet metal part to 'dxf' file? In solidworks, we are exporting the sheet metal flat pattern directly with preview dialog box..

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[MartinHanak]

Abilash,

create a drawing of flat pattern and export it into DXF file.

Martin Hanak

[as-2]

MartinHanak‌ Thanks for your reply..

But Is there any other option in part feature can we export directly to 'dxf' rather than creating a drawing?

[TomD.inPDX]

You can but you don't get the benefits of drawings.

The feature you want to export has to be in the X-Y plane of the selected coordinate system.

[as-2]

Antonius Dirriwachter‌ Thanks sir...

Ya i did the same.. We must scale either flat pattern in drawing or cad file...

Also I came with difficulty of exporting of bulk files.. we must create a individual drawing and the to export.. Is thr any application has been devloped?

[TomD.inPDX]

I typically put all the 3D models in one drawing, one sheet for each part. Make the view 1:1 and use a user defined size to fit the part. I also have to change the color of the lines to 0,0,0 (also user defined) in the options.

In order to make sure the part is at 0,0 in the drawing, I add a point in the lower-left of the part to re-assign the origin of the view. This has worked very well.

[as-2]

Thanks sir...

[JamesKasson · Accepted solution]

"We must scale either flat pattern in drawing or cad file..."

You may set the config option "dxf_out_scale_views" to yes and it will export the drawing sheet at 1:1 scale regardless of view scale. Please note that if you've more than one view on the sheet they must all be the same scale.

[HugoHermans]

We made a mapkey that create a temporary drawing based on drawing template. After the Save As to DXF of that temporary drawing, it's closed without saving, so it doesn't exist anymore. The user has the perception that the DXF is created from the model, but it isn't of course. This way, we are always 100% sure the DXF is 1:1, is without annoying tangent lines etc.