Formatting for CNC router using DXF or DWG file

60158811348__934196E9-8563-4EB5-B25A-0357700B1F51 pantry1Aflattest.dxf (2.8 MB) pantry1Aflattest.skp (332.3 KB) Hello,

I drew up a simple design for a pantry cabinet Sketch up. I’m trying to get the pieces cut by a CNC router. I laid all the panels out on 3d cut sheets that emulate 4’x8’ plywood sheets, The CNC router operator said to send the file over as a .DXF or .DWG file. I can export my cut sheets but the files aren’t working for the CNC. The gentleman said I needed to get the items on the right plane. How do you format for exporting a .DXF or .DWG file that can be used with a CNC router? He said to put it on the right plane and flatten to 2D

Also, I drew rabbet joints on the box panels for the assembling the back piece. How do you leave a partial cut in the plywood panel for the cnc router to read the joints and not just completely cut through the panel?

This is my first Sketchup project but I’m hoping to figure out how to use the program with the CNC router so that I can make several of the same cut sheets at once.

Thanks for any help

From what I’m seeing it would appear the DXF file you exported were in the 3D format. That is, a 3D DXF containing 3D geometry. When I open that DXF file in a 2D CAD program I see the same problems as your screenshot shows. I would guess that is the issue the “gentleman” is having as he needs 2D geometry only by the sounds of it.

There are many answers to your question as all CAM software is capable of different things and the native SketchUp exporter has it’s limitations too.

A few options from what I know:

Option 1: For the quickest fix in this case you could set the camera to a standard “top” view and “parallel projection”, then export a 2d DXF. You then end up with this…

Drawbacks of the above are that the native exporter doesn’t export polylines only singular edges and so the “gentleman” will either have to join the intended toolpaths manually, or the CAM may have a join feature. But I imagine it will be manual labour to create the intended toolpaths from what I’m seeing. Also exporting as a 2D DXF will not preserve true circles and arcs (from SketchUp segmented ones) in the resulting DXF file which might be a personal downside.

Option 2: Would be to export the file as a 3D DXF which would preserve true circles and arcs, but again no polylines. However, seen as though the “gentleman” wants a flat 2d image as it would seem his CAM might not support 3D, I guess that would mean you need to take a copy of the file and manipulate it to put all of the edges on the same plane (ground plane) to make it into a flat image. So that you export a 3D DXF file but it only contains 2D geometry.

Drawbacks of the above: No polylines again. Even though true circles and arcs are preserved, arcs have a bad habit of going rogue and disappearing/flipping when the DXF file is imported into CAM. Myself and other users have experienced this and will take a lot of fixing.

Option 3 (£££): Simple DXF CNC exporter plugin. Which were developed as a result of issues that users were reporting using the native 2d and 3d exporters. It takes some setting up of the parts and getting used to, but exports directional polyline toolpaths and preserves true arcs and circles without issues. It can be used with CAM that supports both 2d and 3d.

Talking 2d DXF, I would make this adjustment in the CAM software in the cut depth or Z height of the operation. There is the more advanced option to set up a layering system. Thus assigning different operations/cut depths/tools to layers which are read in the CAM as such but I’ve never got round to investigating that myself.

After all that, If you’re planning on doing a lot of this I think it’s important to understand the requirements of the CAM software itself and what it can and can’t do to be in with the best chance of success.

CAD software (SU etc.) specifies what the part needs to look like - needs to be done, radius, groove, depth, scoring option etc. etc.

One of the most important aspects is for the CAD software to specify a layer name which is used by the CAM software (Aspire etc.) to determine what tool to use, speed of cut, rpm, number of passes to achieve proper depth, onion skin, tabs etc. etc.

As Ian states - some CAM software can make use of 3D information. In some cases 2D software can determine depth right from the layer name. For example “Shelf_Hole_12”. The CAM software reads the _12 as 12 mm (or uses decimal inches if set up that way)

This can get rather complicated.

Plugins such as CabMaker work with CutMaster which gives you control over all drilling and grooving. Here you can control distance between parts - part rotation - optimized nesting and even cabinet priority processing. You can even adjust the distance between parts for small parts which reduces risk of small parts having insufficient vacuum hold down. Furthermore you can have Cutmaster automatically compensate for edge banding thickness by adjusting part sizing and adjusting relative placement of holes and grooves.