hi all,

ive got a denford traic vmc milling machine which runs on mach3.

ive just received this bad boy -

http://www.ebay.co.uk/itm/230832885828?ssPageName=STRK:MEWAX:IT&_trksid=p3984.m1423.l2649



can anyone give me any info on how to set it up in mach3?

im assuming i need some fancy code to tell the machine when to pull up etc?

Looks like a reversing holder so easiest way (if you have spindle speed feedback) is to use G95 and feed at the required rate for the pitch then reverse the Z at the desired depth.
Hood

ok thanks, to be a pain could you explain a bit further?

ive only owned my mill with mach3 for two months so im very very new to all this

i want to tap m2, m3 and m9 holes

Ok first thing is do you have  spindle speed feedback to Mach? In other words does the RPM of the spindle display correctly in Mach?
If it does then what you would do is change to G95 just before you wanted to start the Z moving down.G95 is feed per rev so you would then command the Z to feed to the depth you want at the feed suitable for the tap.
Example, you would position the tap above the hole then your code would be something like this if the depth you wanted to tap was 10mm and you were using a M3 tap (M3 tap is 0.5mm pitch)

Position above the hole with the code (say 5mm above) then the code for the actual tapping would be
G95
G1Z-10F0.5
G1Z5
G94

Obviously your spindle would have to be running etc but that should be happening with your prior code.
Test cutting air for a while until you are sure it looks fine then test in some soft material. Once you have done it once or twice you wont have to worry

Hood

many thanks for the detailed information.

not sure on the rpm thing, how would i find this out?

i have to set to spindle speed before i can do anything so command s3000, does that mean anything?

If using the standard Mach3 mill screen you will have a DRO that is called RPM, if that you command a spindle speed and switch the spindle on with a M3 or using the screen button then the DRO should start reading the true spindle speed. If it is at zero when the spindle is running then you dont.
Hood

ok ive just been told no spindle feedback, is this going to cause issues with using the tapping head?

It makes it a bit more hit or miss. You should still be able to use G95 to make the feed calculation easier but Mach would just assume that the spindle is revolving at the commanded speed, if its not then the feed would be wrong.
You could also use G94 (feed per minute) but that means the feed has to be calculated with respect to your RPM and then, as before, it would all hinge on how accurate your spindle speed is in relation to the commanded (or calculated) speed.
With a reversing tapper it should be ok as long as you are close or if anything slightly under feeding the Z as the tapper should free wheel if its going down too slow for the spindle speed. Go way to slow and it will reverse as you are going down which you dont want.

Hood

IF you log onto the tapmatic website you will find code examples for their tapping heads (;-) it is a bit different than you think.

Just a thought, (;-) TP

Try here for the CNC Gcode example. I have one of those bad boys sitting in the tool crib. You MAY want to double check the oil in the oil for signs of Coolant contamination and change it out if needed.

http://tapmatic.com/images/pdf/install_instructions.pdf

Just a thought, (;-) TP