Rigid tapping problem

[GITRDUN]

Machine is a 94 VF-1. I bought it used and havent tried using the rigid tap untill now. The processor went bad and we had to install a new processor & board so it lost all the parameter settings and such.
When i tap with it, you get 3 or 4 good parts then all of a sudden it will break the tap while tapping. Whats happening is the spindle and feedrate arent staying 100% in sync with eachother. It varys just enough to snap the tap. Im thinking there is a parameter setting somewhere that has to do with keeping them in sync with eachother. But i dont have the manual for this machine, and the manuals we do have are for 96 and newer machines and dont explain the paramater settings.
Any suggestions apreciated.

[JPMach]

Check parameter #57 the Rigid tap param should be 1. If its a zero and you don't have the original manual you will have to call either your local tech or a factory tech to get the code to enable it.
Are you rigid peck tapping? If so then make sure Setting 133 is turned on. Also if still having problems try putting a 1 in for setting 130 so that the tap pulls out at the same speed as it goes in.

Does the machine have a 2 speed Gear head? What size tap? What material?
If a small tap and a gear head up the rpm of the tapp to the point where it will run it in high gear (I forget the speed at the moment). In high gear it is much easier for the machine to instant reverse, low gear the motor is spinning much faster and takes longer to reverse.

You say a couple parts will come out and then one will break. How secure is the tap in the holder? What hieght above the work are you starting? If you start to close to the work the axis doesn't have enough time to catch up to the spindle. I have had a tap or two pull out of a holder on me far enough so that when the machine moved to the next hole the tap was still in the last one and snap.

JP

[GITRDUN]

This machine is old enough that I dont think it has setting 133 on it.
I dont recall the paramter #, but in order to get it to tap at all, i did have to change the rigid tap parameter from a 1 to a 0 i think. Before changing the parameter it would just sit there on the G84 line with the spindle turning and Z axis wouldnt move at all. What enabling code are you talking about?
I talked to a Haas tech on the phone and he said to check the belt between the tach and the spindle to see if its loose or worn. I took the hood off of the spindle and motor and cant seem to find the tach or belt he was talking about. (starting to wonder if this machine actually has rigid tapping)
The first lot of parts i tapped were 3/8-16 threads in 6061. It ran fine but 25% of the parts had chewed up threads. I set up on some 1/4-28 thread parts made of 1020 steel and tapping only .5" depth. The first part tapped like a dream and the second one broke the tap half way into the part. The problem is without a doubt the syncronization between the spindle and z axis.

[Geof]

I have a feeling your machine does not have rigid tapping and you should be using a floating tap holder to accommodate the slight mismatch between the spindle and the Z feed. We have a '95 Haas lathe that needs floating holders.

[GITRDUN]

Im allready hunting a floating holder just in case i cant get this working right.

[JPMach]

If the extra beltdriven encoder is not there then I would agree with Geof that the machine probably does not have rigid tapping. It would explain why when it was turned on the the spindle just sat there spinning with no movement in Z. It was looking for the encoder signal so it knew how fast to move Z but since there was none it didn't even know the spindle was turning.

Yes you will need a floating tap holder for that machine.

JP

[haascnc]

it sounds like your tach pulley and belt is bad.it has to be there that is how the control know the spindle speed and i think the tach control the tool change position of the spindle .it should be on top of the gear box.i'm pretty sure it is on the left hand side toward the front of the gear box.i don't think they started useing setting 133 until 1998 which multiples the tap retract speed.i have had trouble with that option so i keep that setting at 1 to 1

[GITRDUN]

My machine doesnt use a tach to control the tool change position, its too old. The older machines (before the Vector drive) use a hydraulic pin to orient the spindle for tool change.
I am using a floating holder and it runs fine. Just have to program each move line by line rather than using a G84 command line.

[JPMach]

Originally Posted by GITRDUN Just have to program each move line by line rather than using a G84 command line.

I don't suppose your machine has macros? Then you could at least program a custom macro for tapping with the floating head and just call it up and fill in the location and depth and such.

JP

[JWK42]

I think G84 should work with a floating tap holder. You might have to slow the RPM down or program the hole bottom short to accommodate any coasting to extra depth that a floating holder will do. This would still be better than programing each move. Try it out on a piece of pine 2 x 4 to test it before you break a tap in a good part.