[mvcorrea]

Hi there,

First time milling a pcb.

A situation I have gerber/exellon files for a pcb.
I already drilled the holes (exellon) and worked perfect.
the situation is how I remove the inner circle inside a pad to clear space for solder, from the gerber file (I dont need it as I already drilled the board right?)
I think this is a normal procedure when milling pcb's?

Thanks for your help


I am using a program called flatcam (FlatCAM: PCB Prototyping CAD/CAM) love it. Tried a lot of them.

Attachment 270456

[Bubba]

If I am reading you correctly, you have drilled the through holes. Then there is nothing to worry about as you want the solder to flow around the "pins" and bond to the pad; so less clearance is better!

my .02

[mvcorrea]

Hi Bubba,

I've seeing pictures on the net (included). The board isnt supposed to be like that?m (without the inner circles?)

Attachment 270492


Because when simulating the machine also try to cut the inner circle (after isolation)
I also notice that the inner circle/outer circle+track is the same object (I cannot go there and delete the inner circle)
In my case I only have the gerber/exellon files. So I cannot edit the original eagle/kicad.

Thanks for your help
Marcelo

[Bubba]

I am not familiar with your cam program, but does it have a setting that will allow you to ignore hole sizes <xx????

I use Eagle and the pcb-gcode.ulp

[blinkenlight]

The Gerber format does indeed allow pads to be defined with an internal hole. However, since in isolation milling you normally use Gerber files to mill the isolation contour and Excellon files to actually drill the holes, isolation software normally ignores those pad holes in Gerber files exactly because you don't normally mill them as contours (I just tested this with FlatCAM - holes inside my Gerber pads were not displayed, I had to load up the Excellon file too for the holes to show up). I have no idea why FlatCAM would want to mill them out if that's indeed what's happening - it would help if you could post your file (or even just a small portion of it, if you'd rather not put the whole file on the internet). Anyway, stressing again that this is not supposed to be necessary, there is a simple way to "delete" holes directly from your Gerber files: you just have to use a text editor to open them (Gerbers are actually text files), then look for a bunch of lines like this at the top:

%ADD10C,0.006000X0.003000*%
%ADD11O,0.086600X0.059100X0.030000*%
%ADD12C,0.059100*%

Basically, you're looking for lines beginning with "ADD". The hole itself in the pad is described by the last number in those rows that actually have a hole included - you can just delete the number and the preceding "X". Lines wit "C" codes (circles) must have at least on number (diameter), those with "O" codes (ovals / obrounds) must have two (width and height) and so do "R" ones (rectangle). Anything more is the diameter of the hole, like with my first and second line. De-holed they would look like this:

%ADD10C,0.006000*%
%ADD11O,0.086600X0.059100*%
%ADD12C,0.059100*%

Still - you're not supposed to have to do this. But if nothing else helps, you can easily try it. Good luck!

[mvcorrea]

Hi there Blinkenlight,

Thanks for your reply.
very very very enlightening....
I actually managed on how to find a match but not consistent
Removing/commenting(G04) I managed to remove some pads.
But did not find a pattern to it.

G01X0039248Y0007685D03 <-- outer circle
G04 G01X0038248Y0007685D03 <-- inner circle (x with minus 1000)
G01X0039248Y0006685D03
G04 G01X0038248Y0006685D03
G01X0039248Y0005685D03
G04 G01X0038248Y0005685D03
G01X0039248Y0004685D03
G04 G01X0038248Y0004685D03
G01X0039248Y0003685D03
G04 G01X0038248Y0003685D03
G01X0039248Y0002685D03
G04 G01X0038248Y0002685D03
G01X0039248Y0001685D03
G04 G01X0038248Y0001685D03*

[blinkenlight]

Oh, then it's the much worse case I was afraid of - what you got there is not the kind of Gerber that is used to create PCBs. It is the right type of file of course only with the wrong kind of information in it. The problem is that normally Gerber files represent "the skeleton" of traces and pads (the line down their middle or their center point) - the sort of thing that goes "there is a trace from point X to point Y, Z wide" or "there is a pad at X/Y, with Z diameter". Gerber-capable software then interprets and draws appropriately thick lines and circles. In your case, what you have is apparently not that "conceptual skeleton" described in that Gerber, but the pathways that represent the contour of the already rendered traces and pads, describing them as "draw two parallel lines (the sides of the original trace) ending in a long arc (the pad at the end of it)". It's basically the equivalent of applying a "contour" filter in Photoshop, and it's about as irreversible too.

That's a serious problem, because a) software is accustomed to mill around a Gerber feature, not along it, so it would probably try to mill every single line you see twice (on the "inside" and on the "outside", thinking both sides of your traces being two very thin traces themselves) and b) I'm not aware of any software that can reconstruct the original Gerber from such an "outline of a Gerber" file. Such files obviously have no simple way to "turn off" holes inside pads, since every one is just a circle inside another circle - software can't even tell which one was supposed to be a pad and which one was a hole initially. You really should try to make sure there's absolutely no chance to obtain the proper Gerber files from wherever you got these - making only these available is sort of similar to only giving someone the binaries of a software, but not the source code - this is almost the equivalent to a picture instead of the real thing. Unfortunately, I'm not sure what you can do at this point short of redrawing the whole PCB based on what you see in the Gerber...