Export for cnc file

when i export drawing lines as .dxf or .dwg from rhino, exported files has lots of vertex in CNC software or Autocad special in arc lines, also i convert or simplify lines but there is problem yet. what is the best method to have good result in exporting files for CNC.

Rhino uses wrong default settings for exporting curves into DWG or DXF. That causes lots of problems, such like an unwanted loss of accuracy, overly-dense curve segments, and huge file size. The easy fix is to change those settings as shown below:

It’s recommended to save that scheme so that you can use it every time instead of Rhino’s wrong default settings.


thank you for your helpful guide. i changed the schema as you recommend and the problem solved.

1 Like

Nice to hear it helped for your project. Cheers! :slight_smile:

1 Like

Hi McNeel, Bobi’s defaults seem pretty good. Why don’t you make them everyone’s defaults?



I also think that those settings must be the default ones when it comes to DWG and DXF, because many Rhino users learned it the hard way that Rhino’s default export settings are messing up their work.

@valibeigi.akbar which export setting were you using that caused this excessive amount of curve segments?

I agree, that problem exists at least since V4. V2 and V3 I can’t remember. We could not program our punching machines with the default settings, for conversion to g-code you need clean data. Laser cutting services send us the data back, as they could not use it - data too big for cuttings hundreds of parts from one 3x1,5 m sheet of stainless steel.

I don’t necessarily agree that the “Default” export setting is completely wrong. I think the main problem is that it has curve tessellation checked, which IMO should not be a default setting. Why? Because it does something that is not WYSIWYG - it will segment your curves and you have no idea what the result is unless you reimport the file and check. Plus, that setting might have been appropriate for downstream software back in 1998 when Rhino came out, but 25 years later, it is no longer necessarily the case…

The rest looks OK to me, the “Explode polycurves” setting would be a good subject for discussion, I have dealt with suppliers that like this, as their CNC software wanted simple elements in order to do its own chaining of contours.

Another thing I would add is that “Simplify lines and arcs” - which should be unchecked by default - should have an option “use file tolerance”. Like running Simplify in Rhino before exporting. If it had that option, I might leave it checked. The hard-coded default value of 0.05 doesn’t make much sense to me.

Exporting polylines as splines in not a good option to have as default IMO, we have had problems with other software doing that.


In my experience from producing 10 thousands of parts from Rhino data:
Laser cutting services get a lot of garbage data from all kind of softwares and sometimes just fix the files by drawing a new outline on top of your data without telling you. That can produce some very costly mistakes. Best practice for me:

  1. Check the dwg in Autocad LT or similar
  2. For 2d Data: send a proper pdf drawing with dimensions and tolerances. The guy on the machine can fine tune the cutting path, so you get parts within your tolerances. He just needs something he can manually check. If tolerances are are not met they can put the pieces in their bin. Otherwise you pay and put the parts in your bin.
  3. Also produce a finely tesselated poly line version of your data, so they can check the imported nurbs data vs the poly line version. All sort of weird things can happen on import in a system that converts everything…

O thanks so muuuuch!!! :heart_eyes: