exporting creo drawings to dxf format for manufacturing

[wildmodeler]

Hi guys,
We have a vendor that will only take dxf files for water jet & plasma cutting. We have trouble getting creo to export dxf files with the correct scale. They seem to have a mind of their own. What setting or format should I use to create dxfs that come out 1to1? (I know the vendor should update his software to take a step file but I cant control that.) Thanks for any help

 

[robertib]

There are 2 config options


dxf_out_drawing_scale yes
dxf_out_scale_views yes

 

[srieger]

I usually add a second sheet that is the pattern to be used for export for laser, plasma, water-jet, pressbrake, etc. I place a view of the pattern at 1:1 scale and export. Works fine and is very predictable. Also prevents rounding issues when double scaling using the config options.

 

[KK_designer]

Besides those two config options and scale on the drawing view (wich must be always 1:1) you must check also drawing_units (drawing option) is it in inch or mm.
I usualy make dxf from drawing, save as and pick .dxf extension, and that dxf pull units from current drawint (current config).

I hope it help

 

[michael3130]

I do as srieger does and it works well, this method is used throughout our group of companies. Also do as kk_designer says and check units