ID Groove

will_0000 · Feb 8, 2013

Running a program that requires a number of ID grooves, Groove is 37 ID 44 OD 4.80 wide. Top header in program states 9.5mm minimum bore as there is a small bore at the back of the part, front is bored out to 37.0. When the grooving tool comes in it does so at 9.5mm which will cause a crash with the back of the tool. I want it to come in at clearance to 37. if I program 37 minimum bore it works fine but the rest of the program has illegal cutting points. How do I set the approach size for an ID groove.

Thanks

Will

Lyk31337 · Feb 8, 2013

I believe your machine is much newer than the two I run but if it has a tpc menu it should be able to be set there, or you always could use MNP after all its only one groove.

Or you always could just split the program and have it continue right to the next one for that groove.

Philabuster · Feb 8, 2013

Safest way is to break up the program into two different programs and put the 37mm ID in the top header. This is a bug in the older Mazatrol software at least as early as the T-2, if not the T-1. This same bug also affects ID threading the same way.

The TPC function came out with the T-32 control, so any older control is not going to be able to use it. :bawling:

You can avoid two programs by using the MNP function to groove the bores with G-code. Sucks but it works.

A sketchy (and dangerous) way to fool the old control to make the groove OP work in Mazatrol in one program is to add a dummy drilling operation 37mm dia x .1mm deep after the 9.5mm work is done, but before the grooving OP. The dangerous part is the machine will crash if you restart the program after the dummy drilling OP or if you single process the groove OP.

will_0000 · Feb 12, 2013

Thanks for the information, we ran the groove in its own program in the end. Nice to know the little bugs these controls have. It's a T-2. I haven't tried the MNP function as the lathe is fairly new to us but I will have to have a go.

Bob Wade · Feb 12, 2013

Will

I just had the same problem with the tool backing out too far after each cut and crashing into the back of the tool if i am not mistaken parameter u41 controls the amount of backout in the x axis and u60 in the z axis I found these in our qt10 programming manual and it has a t-2 controll as well. Check it out if it works it will save some headaches.

Bob

Search

Largest Manufacturing Technology Community on the Web

Search

ID Groove

will_0000

Aluminum

Lyk31337

Cast Iron

Philabuster

Diamond

will_0000

Aluminum

Bob Wade

Aluminum

Similar threads