Rookie needs help with Mazatrol T-Plus on QT20

Hey guys - I've been hovering over this site for tips and tricks for quite some time now, and my recent endeavors at work have finally lead me to creating an account for posting. In short, I've been doing CNC work in some capacity for 7 years or so (I've had virtually NO lathe experience), transitioning from button pushing to set ups, to more complex set ups and now programming. I've only known G-code programming for that time, and I'm catching on to Mastercam pretty well, but the Mazatrol is giving me a headache. I guess I understand the basics well enough to get by at this point. All I got before the programmer left was a 10 hour crash course in which he showed me set up, some turning, threading, adding/removing taper. A lot of that stuff is pretty user friendly, but in the last couple days I've generated a couple of questions that I could use help on:

1). I was attempting to tap with an M6x1 .5 in deep the other day, but couldn't figure it out. Do I follow the standard formulas for tapping? I think I was spinning at 200 RPM and feeding 8 in/min. That didn't work very well - I'd get threads at the bottom of the .5 but not at the top of the hole. 200 RPM doesn't seem aggressive to me at all, is it meant to be run a little quicker? Do I need to indicate in my tap when setting up?

2). I had an issue when using the tailstock my rougher would finish it's business and then the turret was returning to home to change to the finisher, which resulted in the finisher coming into Z0. at a sharp angle and the tailstock being in the way. Is it possible to have the turret stay at it's position on Z and just back off on the X for it's change?

Thanks for any help you guys are willing and able to lend me. Thanks for having me, too.

For a feed rate, Mazatrol tap cycles ask for thread pitch ( e.g. 0.05 for a 20 T.P.I. thread), not inches per minute.

On the first line of your program it will ask you the major diameter of your material. Tell it the material is much larger, that should give you clearance in X for a tool change. In addition, if it thinks there is a very long tool in your turret, it will move back in Z until that long tool is now in front of your part to clear for a turret rotation.

Good luck and many fruitful postings!

I do not know a thing about Mazatrol, but you can not feed at any rate other than 1mm/rev with rigid tapping and I would imagine that a tapping cycle should exist if you have that option. Exception being when you use a springloaded tap holder, in which case you can feed a little bit faster on the in and out. Your 8 in/min @200 RPM = 1.0160mm/rev. I would go for 1.2mm/rev on a .5" deep M6 thread and then retract at the same rate.

zoeper said:

I do not know a thing about Mazatrol,

Click to expand...

Mazatrol is a completely different beast than your G code programming. It is all canned cycles. I hate to simplify it too much, but you can call it "fill in the blank" programming. Once again, all Mazatrol threading require a feed per revolution command, not inches per minute.

Gobo said:

For a feed rate, Mazatrol tap cycles ask for thread pitch ( e.g. 0.05 for a 20 T.P.I. thread), not inches per minute.

On the first line of your program it will ask you the major diameter of your material. Tell it the material is much larger, that should give you clearance in X for a tool change. In addition, if it thinks there is a very long tool in your turret, it will move back in Z until that long tool is now in front of your part to clear for a turret rotation.

Good luck and many fruitful postings!

Click to expand...

Thanks for the reply, Gobo!

Only one thing...when I start the line for tapping on my program it asks (going by memory here), type of tap, nominal dia. of tap, pitch, V (below this it says ?in/min), st-pt Z, f-pt. Z. So for the 'V' value I assumed it was asking me for a feedrate and used 8 as I calculated it. What should my value be there if spinning 200 rpm? Or is there a value I plug in to defer?

dodgin said:

Thanks for the reply, Gobo!

So for the 'V' value I assumed it was asking me for a feedrate and used 8 as I calculated it. What should my value be there if spinning 200 rpm? Or is there a value I plug in to defer?

Click to expand...

V is velocity, or in other words, surface footage (cutting speed). The machine will look on your tool data page for the diameter of the tap, and adjust your spindle RPM according to the diameter you entered on your tool page, and the velocity you program in.

Gobo said:

V is velocity, or in other words, surface footage (cutting speed). The machine will look on your tool data page for the diameter of the tap, and adjust your spindle RPM according to the diameter you entered on your tool page, and the velocity you program in.

Click to expand...

Ahhh, okay. So I guess is there any particular way to determine what velocity I need to program in, or is that pretty much dependent on the preference of the programmer or what kind of run you're doing?



Edit: Now that I think about it, the velocity should be programmed higher or lower depending on the max spindle speed I set, correct?

dodgin said:

Ahhh, okay. So I guess is there any particular way to determine what velocity I need to program in, or is that pretty much dependent on the preference of the programmer or what kind of run you're doing?



Edit: Now that I think about it, the velocity should be programmed higher or lower depending on the max spindle speed I set, correct?

Click to expand...

Velocity (surface footage) is determined by several variables. Material, rigidity of fixturing and tooling, and others too numerous to list. Your surface footage for cutting aluminum is going to be much greater than when machining titanium.

For the issue of the tool running into the tail stock, the simple way is to use a 'TPC' or tool path control. After you have completed your tapping unit, return to the starting line of the unit, press the right menu key, and then press 'tpc'. Cursor past the parameter changes to the part that says 'Auto', set to manual, then enter 6.0 for X, 0 for Z, then TPC END. This will make the tool called in this unit travel to 6" diameter, z 0 position before going to the start position. If the finish tool is not the rough tool, you need to change the 'Auto' to Man for the finisher as well.

Gobo said:

Velocity (surface footage) is determined by several variables. Material, rigidity of fixturing and tooling, and others too numerous to list. Your surface footage for cutting aluminum is going to be much greater than when machining titanium.

Click to expand...

Yes, right. Gobo, thanks for all the input. One final question on the tapping, though: On that line of programming when it asks for nominal diameter am I actually plugging in the major diameter after selecting the tap type, and for the pitch am I inputting in MM or IN? Haha, moderately confusing me using metric taps on a Japanese machine where all my other values are in IN. Thanks much for your help.

Red James said:

For the issue of the tool running into the tail stock, the simple way is to use a 'TPC' or tool path control. After you have completed your tapping unit, return to the starting line of the unit, press the right menu key, and then press 'tpc'. Cursor past the parameter changes to the part that says 'Auto', set to manual, then enter 6.0 for X, 0 for Z, then TPC END. This will make the tool called in this unit travel to 6" diameter, z 0 position before going to the start position. If the finish tool is not the rough tool, you need to change the 'Auto' to Man for the finisher as well.

Click to expand...

Oh man, that breaks it down nicely. I'll give it a try and let you know how I fare.

dodgin said:

Yes, right. Gobo, thanks for all the input. One final question on the tapping, though: On that line of programming when it asks for nominal diameter am I actually plugging in the major diameter after selecting the tap type, and for the pitch am I inputting in MM or IN? Haha, moderately confusing me using metric taps on a Japanese machine where all my other values are in IN. Thanks much for your help.

Click to expand...

To program a 1/2 X 13 tapped hole on the face of a part with a T-32 controller-
"Tap" soft key
"Face" soft key
"UNFY" soft key
"Half" soft key- Will highlight pink
Key in "1-13" input button
"Auto set" soft key

Then input your tool number and geometry.
Using your autoset soft key, the machine will automatically set the pitch, and the surface footage according to which material you have chosen in the first line of your program.

dodgin said:

2). I had an issue when using the tailstock my rougher would finish it's business and then the turret was returning to home to change to the finisher, which resulted in the finisher coming into Z0. at a sharp angle and the tailstock being in the way. Is it possible to have the turret stay at it's position on Z and just back off on the X for it's change?

Thanks for any help you guys are willing and able to lend me. Thanks for having me, too.

Click to expand...

You can select Tool change position with parameter P17

Bump.

Hey guys, been doing a lot of work on the Mazak I posted about and I'm really growing attached to the machine. Came back for one more minor piece of advice - does anyone have any suggestions as to where I might be able to purchase some already serrated, blank chuck jaws for my machine? Is there a website anyone can point me to? Google search results super watery.

dodgin said:

Bump.

Hey guys, been doing a lot of work on the Mazak I posted about and I'm really growing attached to the machine. Came back for one more minor piece of advice - does anyone have any suggestions as to where I might be able to purchase some already serrated, blank chuck jaws for my machine? Is there a website anyone can point me to? Google search results super watery.

Click to expand...

Monster Jaws on ebay. Just need to determine what size chuck you have and width of T-slots:

8" Aluminum Soft Jaws 1 5mm x 60° Serrated for Howa Type Lathe Chucks 2 0" HT | eBay

http://www.ebay.com/itm/8-Aluminum-...050?pt=LH_DefaultDomain_0&hash=item53e29aeada

Philabuster said:

Monster Jaws on ebay. Just need to determine what size chuck you have and width of T-slots:

8" Aluminum Soft Jaws 1 5mm x 60° Serrated for Howa Type Lathe Chucks 2 0" HT | eBay

http://www.ebay.com/itm/8-Aluminum-...050?pt=LH_DefaultDomain_0&hash=item53e29aeada

Click to expand...

Awesome, thank you very much.

Is there any formula or rule of thumb when it comes to determining chuck/tailstock pressure? Are there default values for either/both that are safe to keep the machine at?

dodgin said:

2). I had an issue when using the tailstock my rougher would finish it's business and then the turret was returning to home to change to the finisher, which resulted in the finisher coming into Z0. at a sharp angle and the tailstock being in the way. Is it possible to have the turret stay at it's position on Z and just back off on the X for it's change?

Click to expand...

Use the TPC feature. it basically tells the machine relay points to use before it heads back for a tool change. thus preventing tail stock crashes. example. switch tpc from auto to manual and input x6. and z 0. in all 4 fields. then the tool will finish retract to x6.0 and z zero then head to the tool change position effectively avoiding a colision.

Regarding the soft jaws: Get some that comes to a point too. That way you can bore them for small diameter work - Smaller than what the hard jaws and the normal soft jaws can take.
Regarding the tailstock interference: There is a parameter that tells the machine to to the rapid X and Z moves separate: That way the tool always retracts in X first and then moves back in Z. Lots safer when trying out programs too.