[WJ MARK]

hello, Im setting up a machine for a friend and need some speeds and feeds for a fanuc robodrill. Im tapping 3 m3 x .5 holes in 304ss .250 deep thru hole.

some programming examples would be helpful.

Also I get an error when trying to do a g82 ???

[stevo1]

First off what kind of control is on your machine? G82 is a drilling/c-bore cycle not a tapping cycle. You more than likely need to use G84 but your manual should list you’re tapping G-code.

I have never done that fine of a thread before so you will have to get some advise on the proper speed and feed you want to try. I can give you the calculation for it. Example if you want to use a spindle speed of 60. To figure your feed you take the tread pitch of .5mm and convert it to inches then multiple it by the spindle speed. (.5/25.4)*60=1.181. Speed of 60 feed of 1.181. This is of course if you are in inch mode.

Your tap program should look something like this.

G0Z3.
G84X()Y()Z-.25R.2F1.181
X()Y()…location of second tapped hole
X()Y()…3rd
…etc
M30

The Z will be your tapping depth and the R will be your return plane. After the hole is tapped if you want to return to the initial plane of Z3 then insert a G98 into the canned cycle line. If you want it to return to the R-plane of R.2 then use G99 instead. IIRC most fanucs use a default of G98 so you may not use either one depending on what you want.

Stevo

[WJ MARK]

First off what kind of control is on your machine? G82 is a drilling/c-bore cycle not a tapping cycle. You more than likely need to use G84 but your manual should list you’re tapping G-code.

I have never done that fine of a thread before so you will have to get some advise on the proper speed and feed you want to try. I can give you the calculation for it. Example if you want to use a spindle speed of 60. To figure your feed you take the tread pitch of .5mm and convert it to inches then multiple it by the spindle speed. (.5/25.4)*60=1.181. Speed of 60 feed of 1.181. This is of course if you are in inch mode.

Your tap program should look something like this.

G0Z3.
G84X()Y()Z-.25R.2F1.181
X()Y()…location of second tapped hole
X()Y()…3rd
…etc
M30

The Z will be your tapping depth and the R will be your return plane. After the hole is tapped if you want to return to the initial plane of Z3 then insert a G98 into the canned cycle line. If you want it to return to the R-plane of R.2 then use G99 instead. IIRC most fanucs use a default of G98 so you may not use either one depending on what you want.

Stevo

Thanks I got it figured out. I am programming in inches so I needed to convert in inches.

Also the g82 was for drilling a counter bore. I was getting an error because I used a . next to my P value.


Thanks For the input. Also don't forget the m29 s100 before the g84 line.

[stevo1]

Also don't forget the m29 s100 before the g84 line.

Yes you are correct. I have 2 15series fanucs that I have been working on and they have G84.2 which is ridgid tapping mode and the M29 is not needed.

Stevo

[sinha_nsit]

Rigid tapping is possible through parameter setting also:

Rigid tapping with parameter setting
This is one of the methods of using rigid tapping. There is a parameter which can be used to select between the standard mode and the rigid mode of the tapping cycles (provided the machine is capable of doing rigid tapping). On Fanuc 0i control, set parameter 5200#0 (meaning the rightmost bit of parameter number 5200) to 1, for the rigid mode. If the assigned value is 0, the tapping cycles would run in the standard mode. Though spindle start (M03 / M04) need not be commanded in the rigid mode, the spindle speed (i.e., an S-word, say, S1000) must be commanded in some block, before the tapping block.

And there is peck rigid tapping also.