DRW to DXF scale

[blad]

Hello All,

Need some solution for conversion to DXF from DRW.

We are working in Inch. I have all models in Inch and when I am saving Creo drawing in to DXF, my dimension are not correct.

for example. if I have dimension 100 Inch in Creo It becomes 2540 Inch in DXF. So basically my dimensions are multiplying by 25.4 while conversion.

please find attached creo and dxf files for same part.

please give me some solution to this issue.

Thanks

[TomD.inPDX]

Welcome to the forum, Brijesh.

This is not a normal case. I have often exported and re-imported inch based files and it works correctly.

Please make sure that the part file is inch-units; the drawing file is inch-units; and the DXF export is inch-units.

The drawing scale should be a hint as to what the displayed units of the drawing are. Also remember that the drawing exports to DXF as 1:1. Therefore, a scaled view will be according to the drawing's view scale.

If you would like, you can attach the file to a post and someone will have a look at it. I cannot open academic file but I can open full version files in Creo 2.

[blad]

Hello Antonius Dirriwachter,

Thanks for your reply and I checked all units and its in Inch, also scale is 1:1. Also I am trying to attach creo files to this post but I am not able to.

[TomD.inPDX]

You can attach files if you open the Use advanced editor.

How are you importing the file and to what program?

[blad]

I am saving Creo DRW file as DXF file. Then when I am opening that DXF file in Creo or AutoCAD I am getting part with wrong dimension like I explained in first post. I am attaching couple of files so you can review it.

Thank you

[TomD.inPDX]

It looks like your template file is metric, so even though it reports english dimensions, the drawing thinks of itself as metric. Have a look at the view origin on sheet 2.

This always gets me too. It is not easy to mix metric and english templates in Creo.

When I open a new drawing using an english template (or default empty), the export DXF is 1:1.

[blad]

You are right I have templates in Metric. Is there any way I can change all metric drawings in to english.thank you

[MartinHanak]

Brijesh,

I opened your drawing and did some tests.

1.] In the drawing drawing_units option is set to mm

2.] I exported t001979_mm.dxf file and opened it in CR2 M030 without problems (File > Save a Copy > select DXF format > use default setting for ACAD 2007 format)

3.] Your DXF file does not contain drawing format, it contains only 1 rectangle. How did you create this DXF file ?

Martin Hanak

[blad]

Hello Martin Thanks for your time on this issue.

1. I did change this drawing_units in to Inch but with that I need to chnge properties of arrow, dimensions scale, etc. If I change this in Inch my sheet is full of bigger size arrows and dimensions. Is it the only way??

2. I opened your dxf file but dimension are not matching.

3. I removed format because this kind of part is for machine so I dont need to have format.

I save as DRW file and select DXF to create this dxf file.

thank you

[MartinHanak · Accepted solution]

Brijesh,

I apologize ... my first response had to be confusing for you.

1.] I opened the drawing and modified detail settings using the following procedure

File > Prepare > Drawing Properties > Detail Options > change > click Open a configuration file button and choose DTL file

Some DTL files are located in Creo 2.0\Common Files\M030\creo_standards\draw_standards directory, I used standard_in.dtl in my test.

2.] My first DXF file was wrong because I missed that your view has the scale 0.075.

To output this view in 1:1 scale I set config.pro option dxf_out_scale_views yes

3.] I turned drawing format off and exported t001979_z01.dxf file. It contains $INSUNITS set to 1 (inches). Therefore I hope it is correct .

Martin Hanak

[blad]

Hey Martin,

It worked great using standard_in.dtl...Thanks a bunch for this helpful information.

Hv a good day

Brijesh

[Dale_Rosema]

Don't forget to mark the correct answer for those read the post later.

[ymanoharan]

Hi Martinhanak,

very useful info, thanks it solved my issue also.