milling a circuitboard using the haas nc minimill

author: guy at media

back to topic

this document assumes that you have created your circuit layout similar to the way described in the modeal circuit milling page. here, we will only describe the specific cam.py parameters for the haas operation.

a word of warning

this can probably not be said enough: you will be software-driving a very strong, very heavy, very fast tool that can easily kill people, including yourself, and damage itself and other equipment around it. accordingly...

learn the location of the emergency stop button blind.

do not do anything without the mill-door closed.

always wear safety glasses.

acquire the patience needed for dry runs and simulations.

finally, always keep in mind a picture of yourself with a giant hole in your forehead.

creating the g-code

use cam.py to greate g-code for the mill

Run the current cam.py script, and set the parameters to the ones in the screenshot below

export the g-code

cam.py should output the correct G-Code when the output file has a ".g" extension.

Take a look at the G-Code in a text editor and make sure that the basic sanity checks hold true:

• the file should start with O1234
• the tool you choose should be tool #1 - this is indicated by the line T1M06
• then a line saying G90G54 should indicate that you're using absolute part coordinates
• finally make sure the spindle speed and feed rate are correct (lines starting with S and F respectively)

the choice of tools is very important. the haas mill is not very smart about knowing its own limits (in more ways than one). you definitely do not want to think you're using tool nr.1 - a small 10mil mill, while your G-CODE actually points the mill to use a 5'' drill.

at this point you might want to add a comment in the gcode to mark your file as yours (comments are any text enclosed in parantheses, like this very sentence), this way you can make sure you're running the right file when you load it onto the haas

now save your file onto a diskette and go towards the mill

mill it!

thanks to zeynep for her original step-by-step guide

prepare the stock

• Double stick your copper piece onto the metal base.
• Take the mill spacers from the red box and place your piece on them in the haas. Choose the mill spacers such that your piece&base fit smoothly between the blocks.
• Press tight from both sides.

prepare the mill

• power up the mill. there will be an alarm. this is ok, just press the POWER UP RESTARTbutton.
• make sure that the right end mill is in tool #1
• Put in the floppy. go into EDIT mode.
• Pressing F1 pops up the menu. goto I/O -> Receive Disk. It will ask you the enter the filename. Enter the g- code file name. It will load it. make sure that you're working on your file (see comment above). You can press reset anytime to clear whatever you were doing.

run a simulation

• zero out the origin: hit offset twice, scroll down to G54 and press 'parts set 0' three times (one for each axis)
• go into MEM mode
• press SETNG GRPH(or something similar) twice to get into simulation mode.
• press cycle start to see the toolpath

run the real thing

• go into EDIT mode (i think)
• Set origin: Press Hand jog. At this point if you can't seem to move the head using the wheel on the panel, you want to press power up restart button. Using the wheel bring the head to the x, y, z you want as your origin. TO set z, insert a piece of paper between the mill and the board and slowly get the z position lower until you feel the paper caught between the mill and the stock.
• To actually set your new origin, hit offset twice, scroll down to G54 and press 'parts set 0' three times (one for each axis)
• Now you're ready to go. Get into MEM mode, press DISPLAY CURRENT COMMANDS for a new view of all the parameters, and hit CYCLE START

at any point you can increase or decrease the feed rate and spindle speed by a percentage

You can always stop and air the board to see the progress. Otherwise it's hard to see while it's operating. The following are the steps to stop and check: Press Feed Hold. Press spindle stop. Press Edit. Open the glass window and blow some air. To restart make sure you press spindle CW (clockwise) first and then press start cycle.

more information

zeynep adds

So there is good news and not so good news regarding board milling on the HAAS. Good news is that the final product looks great. (or will do...it's still going - half way through rastering) Very clean contours and rasters. None of the unexpected tapering of lines or messy rastering. The not so good news is that it doesn't take that much less time than modela, at least with the feeds that Manu and I used. So here are a few tips:

• When you are cutting the copper piece to place on the base, do NOT use the shear & break tool. It curves the piece and causes uneven z values, which means parts of the board do not get milled. Always use band saw to cut the right size.
• The acrylic base for the piece was a bit too flexible. When pressed to sit tight it would curve. I ended up using a metal base that Manu gave me - he said he'd make another one.
• I used a raster overlap of 0.7 - I think one could definitely use a higher one (0.8 or 0.85) and that way it'd go a little faster.
• I used a z-down of 0.013: if the piece is flat 0.010 should be good.
• I used a spindle speed of 5000 and feed 5. I did two contours with 110% spindle speed and 90% feed - during rastering we increased the feed up to 120%.

for those who will be milling boards on the haas: it seems like there may be a problem with doing more than two contours on cam.py - Jamie tried N=4 or 5 (don't remember) and had broken traces. Ben (dalton) tried N=4 and had some broken traces. I made two boards, the first was with N=2 and rastering, it came out fine. the second one had N=4 + rastering - that one had broken traces. The moral of the story: Don't do more than two contours.

shelly adds

my five cents

160% feed rate for the rastering, with 0.75 raster overlap works well.

in this case, that's 160% of 5.000 (i.e. effective feed rate: 8.000)

If the endmill breaks in the middle of the operation you can just erase the part of the G code it already went through (I left the very first few lines, though). the location information is absolute (with respect to the origin you set), and not relative to the previous location, which allows you to do that. easiest is to do it on the computer, resave onto the floppy and run the new code. deleting on the HAAS takes ages.

jamie water-jet cut a new aluminum block onto which you can double-side tape your board.