Hi All,

I am making just for fun a optics breadboard. It is just a slab of 6061 with 8/32 tapped holes every 1/2 inch. For the first little one i am building it is 15 x15 grid of holes that works out to 225 holes to tap. My wrist hurts just thinking about it. I could do the old tap in the cordless drill trick but i was hoping to get them all straight and would like to figure out a way to do it on the mill.

I have a grex so rigid tapping is out of the question. I do have a cheapish auto reversing head that I can use in the mill but the problem is it reverses out at 1.75 times the down speed. The other problem it takes about 1 inch to engage the reverse gear.

So I would need a way to set up the grid, feed in at the pitch/rpm to the correct depth, rapid up about an inch then feed out at 1.75 times the pitch/rpm.  yuck.

Any one have any ideas??

thanks
Chad

This would be a great addition to the drilling operations wizards Brian? lol

Hi chad,

 just have a look at this topic, the gcode is for doing just what you want,

you will have to change the feed rates to match your tap and the L words to match your line count and that will work

Graham.

G20 G40 (standard setup lines)
S300 M3
M8
G00 G43 H3 Z1.00
G00 X0 Y0    (set position of first hole as X0 Y0)
M98 P1000 L15 (repeat 15 times)
M30

O1000
(this bit moves Y axis)
M98 P1001 L15 (repeat 15 times)
G91 (set to move incremental)
G00 Y-.5 (do move of .5 inch)
G90 X0 (set to absolute and go back to start of line)
M99

O1001
(this bit moves X axis)
M98 P1002 (tap hole)
G91 (set to incremental)
G00 X-.5 (do move of .5 inch)
G90 (back to absolute)
M99

O1002
(this bit taps hole)
G00 Z.25 (start height for tapping)
G01 Z-.25 F9.375 (feed in depth)
Z.75 F100. (you may need to play with the Z and F figures to engage reverse)
Z1. 5 F16.406 (feed out at 1.75 times in feed)  (remove this line to drill holes and change feed and depth)
M99

AAAH I forgot about that, i remember reading this back when...


Thanks !!

I will give it a try tomorrow.

Chad

Hi Chad,

no problem, I have done a mod to the tapping code based on the user feed back, last time it was used, the person did 570 holes with out a problem.

Graham.

HI Graham I just tried it at home on mach without a machine hooked up just to watch what happened on the dro's. It went through one iteration of the z but the x and y didn't move? I just copy and pasted what you wrote?

I just looked at the m codes list and it says that P is dwell time in a sub..  I must be missing something.

BTW I am not a g code guy at all. I understand some stuff but a lot is just gobblety-gook.  Do you know of any good g code for noobies info?

CHad

Try changing the L's to Q's, Brian says that Mach uses Q not l's

As for the Gcode, just ask me and I will tell you what you want to know, I have been writing Gcode for 2,3,4 and 5 axis for nearly 30 years

Graham.

Hmmm nope, same thing.

Thanks for the offer on the g code, i really would like to get some basics down.

Thanks

Chad

This is what I get using the code :-

Make sure you have a CR after the M99 on the last line of code

Graham.

That was it..   That little chr$(12) would have caused me no end of frustration.

Oh yea, what does the p1000,1001,1002 do? Is that like a goto O1001 and then the m99 a return ( sorry for the old basic references)

Looks great thanks again!!!

Chad

M98 P1001 is a call to a sub program the Pnnnn is the sub program you want to call

The Lnn is the number of times you want to call the sub

M99 is return to the calling program.

Graham.