Rhino to Acad to DXF

[Karsten Sell]

I need some help.
I use Rhino for my design / fairing etc. Then flatten all panels and export to
ACAD. I then tidy up and nest all panels onto sheet sizes (alloy) ready for CNC cutting.
All this works very well and have had some great outcomes.

The problem is that the DXF cutting files have a huge amount of "data" and are extreemly large (about 1 - 2 meg per alloy sheet). I am told that this would / should normally only be around the 150 - 200 kb ???

For some reson the size of the file is causing some problems with the CNC software and requires quite a bit of stuffing around.

Thanks
Karsten

[RThompson]

Hi Karsten,

The first thing that springs to mind:

Are you exporting (from Rhino) curves or surfaces?

Ie When you say "export to ACAD" are you exporting the surfaces themselves or are you exporting curves you have derived from the surfaces.

The surfaces will make the .dxf files much larger.

Rob

[CGN]

Try extracting the edge from the expanded plate in rhino and export only the extracted edge and only markings that you need on your plate (stations and some plate notes), this should result in smaller size of the files, I'm guessing that you are exporting all the "extra" lines that are part of the surface maybe that's why your file are quite large

cheers

[Raggi_Thor]

You have some settings for accuracy when you export dxf from Rhino. Try to increase the segment length og polylines or the max angle between segments, but be sure it still looks smoth in AutoCAD.

[RThompson]

Just another thought I had re exporting from Rhino to ACad for CNC:

Once you have created the panel shape you wish to cut, and laid it flat:

Use "Duplicate Border" to create a an outline shape of the panel.

On the "Curve tools" toolbar there is a tool called "Convert to Arc/Polyline"
Use this tool on your outline shape to convert it to Arc's (obviously setting the toleramces to suit)
- play with it a bit to find whats good for you. I use CNC to cut MDF frames for strip planking, settings I use are
OutPut= Arcs
AngleTolerance=1.0
Tolerance=0.2

You can then export the resultant curve shape.
If you don't convert it to arc's first then on export all your lovely curved lines will be converted to lots of short straight lines = larger file and also slower CNC times.

Rob