Printable View
Hi guys 0/ some of you may have read a post I made about cheap PCB’s. I have my schematic done and working on a proto board. The question is I need to shape the corners and reduce the length of the PCB’s, it has to fit inside a rizla tin :) what recommendations would you have for doing this on the CNC , tooling etc? I’m going to have 2 holes in the PCB so I can locate it on a jig for accuracy.
This might be better off in general CNC but I thought I would start here. :confusion:
to cut FR4/copper clad board on a cnc machine (eg the outline), I use a chip cutter....
10x Carbide PCB Print Circuit Board End Mill Endmill 2.0mm for CNC / PCB Cutting | eBay
(though I use smaller diameters...1.6mm & 1.2mm)
To do the board outline & ensure it aligns with the tracks & mount holes.
1. Create a DXF of the board including mountholes in your favourite CAD app (ie get your rizla tin, measure it up...create your board outline from your measurements with mount hole locations etc)
2. Use an app called DXF to Script converter (google it)...convert your DXF file to an eagle script file.
3. Within eagle 'board view' run the script you just created in step 2 (file ->script browse for the file you created & run it)
Voila....you've now got your exact outline on the Eagle Dimension layer...now you can route your Eagle PCB tracks around knowing with 100% certainty that everything will come out right!
Once you've finished your Eagle PCB layout...
Run an eagle job to save pcb track outlines as a gerber (within board layout, file-> cam processor->file->open->job select gerb274x.cam then process job - this creates a gerber file of your pcb tracks)
Now open up the gerber file in cambam (this is your pcb tracks), convert from imperial to metric (within cambam ctrl A, ctrl e-> select convert from inches to mm) ....it can all be cam'ed up now (along with your earlier DXF file for the outline mount holes)
As ever Hank Awesome , thanks :) I have ordered some 2mm ones 10 should last me a while I post results but it will be a while before I actually do some.
I do mine same as Hank up to the point of getting it out of Eagle.
Here, I use the pcb-gcode.ulp to create the gcode files directly. Then I run Daedelus's Autolevel program to take care of variations in height and run these programs directly on my router. First doing the "etching", then drilling, and finally the Milling to remove the board.
You can use your favorite units system directly with no conversions needed.
Quote:
Originally Posted by C_Bubba
I use CNC-USB (vs Mach3) as it has this Z probling/correction feature built in.
Can you add a bit more meat here? (not fully understanding what you're getting at ...do you mean with gerber conversion? I convert gerbers from imperial to metric as I've not found a way of getting Eagle to export gerbers in metric yet! That said it's only a 30 second overhead to do the conversion)Quote:
Originally Posted by C_Bubba
I do NO gerber output. Pcb-gcode directly exports gcode file(s). You can set it up to do files for top and or bottom for drilling, etching, milling etc. It will do it directly in metric if that is the unit system that you have chosen to use.
As your system has "warp", the files will be ready to run. No further cam work will be needed.
I don't think there is a pp for your controller yet, but it should not be to difficult to massage one of the existing ones. I personally use Turbocnc and have mangled the heck out of the stock pp's:})
I’m only actually cutting the PCB’s out after they have been manufactured; luckily my board size is 48 x 92 so If I get two prints on a single 10 x 10cm I will get two boards out of them. But the corners are rounded and I have to get the board right up to the ends of the tin because some parts go through the metal, so I’ll cut the shape out, should look good hopefully and if my calculations are correct Scotty! Will cost 89p each.. bargain!
Ok, now I get your approach - I prefer having the whole engraving, cutting/drilling CNC aspect in one layered CAMBAM file (vs loading up separate g-code files into a CNC app to do a full pcb job), that why I export a gerber from eagle & bring the track outlines into cambam - I also found the pcb-g-code a bit restrictive (I need to get deep down & dirty with all my parts! For example sometime I need to mill out a bit of waste copper to aid soldering (& avoid bridges) - I can do that easily & see the results prior to going to the CNC machine if I have all aspects of the job in one central app.Quote:
Originally Posted by C_Bubba
If you want a perfect, fantastic circuit board that is cut really well, I suggest you use something called Autoleveller. AutoLeveller - The height adjusting CNC software
Using a simple probe system like a croc clip attached to your machine, you can use your tool to probe the height of your PCB before cutting to get an accurate cut depth.
Simply get your g-code file from whatever your CAM output software is, import it into Autoleveller and it will automatically, based on your variables, edit the g-code to include a probe system before routing the board.
It is very clever and completely free.
Personally, I donated a fiver to the software designer as it's one of the best pieces of software I have used for cutting circuits.
booski , when you say a simple probe what do you mean ? What do you attach the other end of the croc clip to ? I couldnt see any notes on actually setting up the hardware on the site .
The cutting booski refers to is achieving a constant depth (thereby catering for bulges & valleys on your copper board as it isolates your pcb tracks)...that's what autolevellers do.Quote:
Originally Posted by Fivetide
i use CNC-USB (which has autolevelling built in), but there are other flavours out & about (indeed there was a thread discussing one that a memeber here had done a week or two ago)
Yeah, pretty much. I just tape a piece of wire to the board with a bit of tape and then a croc clip to my spindle. The software then probes the height of the board.
How does the feedback of the tip and croc clip get back to the computer ?Quote:
Originally Posted by booski
Well, I have a simple parallel port chinese TB6560 controller and I use one of the input pins on the controller setup in LinuxCNC as a probe. There are 5 input pins on my controller and 1 common, so with a lead connected to the common and another connected to the input.
With the probe attached to the tool, the Z axis comes down and when the tool makes contact with the board, it measures the height and adjusts the rest of the g-code to suit the board at that point.
which is fine until you forget to remove the croc clip before cutting :) . Also a solid tool rather than a sprung 'plunger' means the Z-travel, and therefore the mapping speed, has to be much slower to avoid damaging the copper surface... but it works....Quote:
Originally Posted by booski
Is there any setup instructions for the probe ?Quote:
Originally Posted by booski
Haha, yeah, must remember to remove the probe.Quote:
Originally Posted by irving2008
Fortunately, my DIY spindle motor has pillars holding the motor and so is directly connected to the tool so I haven't got to worry about removing the croc clip.
The autoleveller software if I remember correctly allows you to set the probing speed which default is 100mm/m I think so it's very slow and the machine reacts quick enough that it doesn't damage the board. Similarly, I set the retract height to 1mm so that it retracts quickly and moves to the next point quicker. Could even set it to much less than that really for quick probing.