Results 1 to 8 of 8
Thread: Rigid Tapping on all CNC lathes?
02-13-2009, 12:08 PM #1
Rigid Tapping on all CNC lathes?
We have quite a few questions about having rigid tapping on certain lathes.
Is there really any difference, except convenience, to make up your own cycle using G32 or G33?
I can remember way back, I was training a small shop in Florence, SC, he had a Wasino Gangturn and the job we set up had a 1/4-20 tap in Alum.
There was no Rigid tapping in those days and we programmed:
G0 X0 Z.2*
G32 Z-.7 F.05 M5*
G32 Z.2 F.05 M4*
G0 X2.0 Z2.0*
His machine read the M5 at the end of the line, you would have to check how your machine is set up,
We held the tap solid, no floating tap holder.
Since then, I have than this on a number of different lathes, it seems to be just like rigid tapping.
All lathes have a sort of resolver that coordinates the RPM with the feedrate, mills do not have this, so Rigid tapping is a somewhat costly options.
02-13-2009, 12:14 PM #2
That is the cycle I use on a Fanuc 0T-C but my M5 is on a separate line, I notice with a floating holder there is some extension when the reverse starts. I shall try it with the M5 at the end of the first g32 line and see if the holder extends.
02-13-2009, 03:06 PM #3
The rigid tapping code has the advantage that you can tap faster, since the reversal will occur with a better deceleration, instead of a quick stop.
I agree that any cnc lathe has a resolver for that, but if the rigid tap function is present, it means in the first place that the machine has a better encoder probably.
I prefer to rigid tap because of equal torque reversal.
I always imagine the break test with my car, driving 5mph, kick the break short and hard and im rolling back.
Gotta make sure that my seatbelt is tight.
Somehow i just think that its better for the machine to use it when its there.
And the cycle is a bit shorter
02-13-2009, 04:01 PM #4
This is related to tapping on a lathe,
If you want to peck drill your tapping hole, and you dont have the G83/G81 cycles enabled, is'nt there a way of using G74 face grooving as a peck drilling cycle rather than having to write the cycle out long hand in G01/G00 code
I'm sure I heard someone say it was possible
02-13-2009, 04:16 PM #5
G0 X0 Z..
G74X0 Z-1 P0000 Q... F....
02-13-2009, 04:23 PM #6
On an oldy style fanook, with 2x line G74 code:-
G74 R(retract amount for breaking the swarf)
G74 Z_ Q(infeed amount per peck) F(feed)
This works a treat.
We have also used it for a boring cyle in nylon to get it chipping, by putting the x in for the offsett and a small Q amount.
The tool then goes in / retract & in / retract breaking the chips up nicely.
I was going to try it on an OD on nylon but we sold the lathe and got a siemens,
which has an inbuilt option which stutters the feed breaking the swarf anyway (really neat).
02-13-2009, 05:05 PM #7
02-14-2009, 12:59 AM #8
Rigid Tapping on all CNC lathes?
We really got away from the original subject here, did'nt we.
By the way, the simple use of the G74 is peck drilling, no pullout all the way to clear the part, just a simple retract before drilling deeper.
The more complicated use is as a face grooving cycle that can do a wide face groove in 1 line on older controls and in 2 lines on the 0 series and later controls.
I am not sure I have an example on my website( www.doccnc.com ), if someone needs it, I will post an example.
By the way, this is one of those Fanuc features that is not really explained in any of their manuals.