Eagle 3D PCBs with Alibre: More on Creating DXFs
I mentioned in the previous post in this series that you cannot use the standard Eagle DXF ULP to generate DXF files that Alibre can use.Â Now I will go into a little more detail.
All the files DXF files I mention are available in a ZIP file here Extrude Alibre.zip
What are the problems with the normal DXF ULP?
- It creates the pads, not the drill holes.Â The picture below shows, in green, the pads created by the normal DXF ULP.Â I added the drill diameters in white using DoubleCAD.
- Notice the greenÂ squares (which I use for pin 1).Â I haven’t seen a square drill bit yet…
- Notice the the green square and green circle are much larger than the white circle.Â This is because the DXF ULP is creating the pad outline; for each pad, Eagle adds some copper area around the drill diameter (how much depends on the active design rules).Â Â But we want to extrude the actual hole size through the PCB, not the pad (drill area + copper area).
- You can get around this by creating a special set of design rules that does things like set all pad shapes to circular, pad size to the drill size, etc.Â And you’d better remember to re-apply your normal design rules (or you’ll end up with a worthless board).Â This approach will work OK for SolidWorks (I’ve tried it), but still doesn’t work with Alibre, because of other problems listed below.
- The DXF ULP creates the pads using object blocks (with different blocks for the different pad shapes).
- The ULP creates two identical blocks right on top of each other on the same layer (17, Pads).Â Alibre will not extrude sketches with overlapping objects.
- For some reason, Alibre does not copy the blocks correctly.Â When I imported the DXF into Alibre, they appeared at the right location, but when I copied the sketch to the new Alibre part, they moved to a totally wrong location.Â The picture below shows this with the DXF (Extrude-Different Layers.DXF) on the leftÂ and the part (Extrude-Different Layers.AD_PART) on the right — the pads have moved far to the right.
So what did I do?Â Well, I didn’t have a lot of time, and I’m not a DXF expert, so I made the minimum changed required for Alibre to work:
- I changed the Via function to always create a circle with the drill diameter on the dimension layer (layer 20).
- I changed the Pad function to always create a circle with the drill diameter on the dimension layer.
So far these changes have worked for me, but I should note that AutoCAD 2000 doesn’t like my changes (I haven’t tried newer versions).
The final topic: a bit on the DXF ULP options.
- Output file is the name of the DXF file that will be created.
- Always vector font should force a vector font to be used, but I haven’t test this feature.
- Unit selects whether to use inches or millimeters.Â Always remember the units you choose, because when you import a DXF into Alibre Design, Alibre needs to what units you used.
- Below I show the same simple board creating DXFs using 1) no wire wire or fill areas, 2) using the wire width option only, and 3) using the wire width and fill areas options.Â For extruding PCBs, you should never select the Use wire width or Fill areas options.