We use cookies to personalize content, interact with our analytics companies, advertising networks and cooperatives, and demographic companies, provide social media features, and to analyze our traffic. Our social media, advertising and analytics partners may combine it with other information that you’ve provided to them or that they’ve collected from your use of their services. Learn more.
Sorry I’m running into a frustrating problem that others may have run into. My Excellon file doesn’t line up correctly with my gerber file. I have already scaled it (by 0.01) according to John’s Tutorial (PCB Milling on X-Carve | Inventables) and I have confirmed there are at least 5 digits for the X & Y values but it looks like the placement is still completely wrong. I have tried rotating, upside-down, mirror and various combinations but nothing seems to work.
I do not have a problem when using the eagle FTDI file from John’s tutorial and was able to plot both in flatcam without any problems, it’s just a problem in the PCB I designed. So it seems like a setting problem in Eagle.
Above is a screen shot from Flatcam. The red dots are from the excellon file and the green is the top layer gerber file (each of the pads are through hole). The odd part is the clump of red dots in the bottom left hand corner that seem very out of place. Any help would be appreciated.
I was able to figure out the solution. It appears there are multiple problems in the tool path so I’ve included my solution below in case anyone else runs into this problem. The general problem is you have multiple drill sizes in the excellon generated file (this can be because the components you are using may have slightly different drill sizes specified).
Solution:
Part 1 : In Eagle:
File->Run ULP and select drillcfg.ulp
In the drill size prompt (i.e. T01, T02, etc), leave the T value that you want and remove the rest. In my case I left T01C0.813 but removed T02C1.016
Save the configuration file
Run Cam Processor
In Device, select “Excellon Rack”
For Rack, select your saved configuration file (this will change all your components to that drill size)
You may need to adjust the drill tolerance. In my case I just used a tolerance of 100% to 100% (these were just my test values, I haven’t gone back to figure out the exact values yet).
Run Process Job
Part 2: Altering the Eagle File
In some cases the generated file may not be parseable by Flatcam. If you run into this parse error when importing into Flatcam, follow the instructions below.
Eagle generates two files: DRI File and the file you specify (this is has whatever extension you gave it and can be referred to as the DRD file). Open up the DRD file in a text editor.
If the first two lines of that file are similar to below (then you need to alter the file):
%
T01
To alter the file you need to add the following lines above the % T01:
%
M48
M71
T01C0.813
The T01C0.813 is my drill size, but if you have a different drill size just change it to be T01C. The M48 and M71 are commands that are required.
This is what the file will look like after the alteration:
%
M48
M71
T01C0.813
%
T01
Save the file and import into flatcam.
Also, after you have imported the file in flatcam, selected the file and clicked on the “Selected” tab, the scale factor may not be 0.1 so you may need to play around with the value. In my case, I had to use a scale factor of 0.254.
I put together a little video explaining the manual editing of an Excellon drill hole file for proper importing to Flatcam. Specifically, I am using Eagle 7.4.0 and Flatcam 8.4.
Editing the excellon file allows the user to maintain full resolution and use multiple tool sizes.
Actually it’s non-compliant output from Eagle. The FlatCAM Manual has a section specifically on how to import from Eagle: FlatCAM Manual: “Eagle How-to”.
