Mazatrol T32-3 EIA programming codes for live tooling and C axis

rbmgf7 · Jan 6, 2023

We have a really old Mazak 28M-SQT that was operated forever by one guy using Mazatrol and the operator unfortunately passed away last year.

The machine sat since no one else was versed in Mazatrol until we found out it can run G-Code.

We managed switch to EIA but was wondering what codes are needed to run the live tooling and C axis? Manuals aren't to be found and the online searches are sparse. Thanks.

Skubeesnak · Jan 8, 2023

See if this helps. https://www.practicalmachinist.com/...ing-codes-for-live-tooling-and-c-axis.409192/

rbmgf7 · Jan 9, 2023

Skubeesnak said:
See if this helps. https://www.practicalmachinist.com/...ing-codes-for-live-tooling-and-c-axis.409192/

You linked this thread.

rbmgf7 · Jan 9, 2023

So far I can manage to turn on the tool but I can't get it to feedrate.

I just been writing some arbitrary code to figure it out between the C axis and locking the spindle and so far this is what I have:

G0 X0 Z0
M212
G0C0
M200
M210
S2000 M13
G1 Z-1. F.001
G0 Z1.
M15
G0 X1.
M212
C0
M30

It'll stop at the G1 but if I erase it, it just rapids and continues.

Next, how do you do a drill cycle? I've been dumping milling type code like G99G94G81R--Z--F-- then some C moves and it just gives an illegal G code error.

chad883 · Jan 9, 2023

This is from my T-Plus control. The G83 drill cycle may have been an option on your control.

T0404.03G0G40G98(3/8 X 90 MILL DRILL)
M8
M200 (engage c axis)
G97M203S2000 (turn on live tool)
G0C0.
G0Z.1
X1.25
G83Z-.075Q.4F20.
H120. (index c axis 120 deg incremental)
H120.
G80
M205 (live spindle stop)
M202 (disengage c axis)
G0Z6.0
G4P1000
M1

rbmgf7 · Jan 9, 2023

Once I get to G83, I get a 744 error "no designated program". I tried rewriting it G81R--Z--F and it gives the same error. Guessing I'm missing a parameter? We don't have any manuals (not surprising as this machine is form 1994).

chad883 · Jan 9, 2023

My guess would be that you don't have the G8x canned cycles. I have a 1994 SQT that doesn't have them.
Try changing G83 to
G1 Z-.xxx F10.
G0 Z.1
H120.
G1 Z -.xxx
G0Z.1

rbmgf7 · Jan 10, 2023

Hmm, weird. It doesn't recognize feedrates. It stops on the G1 line but doesn't throw an error. Tried G01 just in case of formatting and no change. I put G94 at F1.,it throws a "744 no designated program error" but when I put G95 at F.001 it says "708 illegal G code".

I found our regional Mazak number so I'll give them a call and hope they can tell me what's going on.

chad883 · Jan 10, 2023

Make sure you are in G98. That is feed per minute.

ViktorS · Jan 10, 2023

This was your program:

G0 X0 Z0
M212
G0C0
M200
M210
S2000 M13
G1 Z-1. F.001
G0 Z1.
M15
G0 X1.
M212
C0
M30

You will never get any feed with that low feedrate. Typo?

Also, write that line as
G98 G1 Z-1. Fxxx

to go into F/min mode. Otherwise it will probably try to use the G99 F/rev mode and the spindle (turning spindle in this case) is stationary so no feed happens.

EDIT:
Also, M210 is C axis clamp, M212 is unclamped/only servo holding. M211 is brake, which applies a friction brake to the axis to reduce harmonics when doing heavy milling. To be able to move C axis the spindle needs to be in either M212 or M211.

(Some machines might not have a brake only-option? Try it and see what it does)

rbmgf7 · Jan 10, 2023

I tried both G98/99 with respective feedrates at either F10./F.001. Position screen doesn't show any Z movement. Erase G1 and it just rapids regardless of the F value.

Philabuster · Jan 11, 2023

How about learning to run the machine in Mazatrol? It is WAY easier than G-coding the thing. I have a YouTube channel dedicated to programming Mazatrol if you are interested. There are a few examples of C-axis milling videos:

https://www.youtube.com/@mazatroltipsandtricks6816

rbmgf7 · Jan 11, 2023

Since we know Gcode, we figure it was faster to get the machine going if we could get the right codes. In actuality, this machine would be best suited for Mazatrol since it was used for the one-piece orders. We just need to try and get things going at the moment. Our local Mazak supporter offered training as well.

ViktorS · Jan 11, 2023

Hmm that IS crazy..
Maby not in the right mode?
I know that Fusion controls at least have two different EIA modes, one of them is called T32 mode.

They use different set of codes. Might be worth looking in to?

noname777 · Jan 12, 2023

Everything is in PARAMETERS MANUAL

rbmgf7 · Jan 12, 2023

We got it. Operator remembered the codes show up in the upper right hand corner of the screen when you're using Mazatrol. We can run Mazatrol just can't program until we get some training (trying to break these people free from being button pushers).

Seems the solution is M248 which I found to be called "spindle speed check for interlocking the start of cutting".

So our simple program that finally ran is:

T0101
G0Z0C0
G98M203S2000
M210
M248
G1Z-1F10
G0Z0
M212
C180
M210
G1Z-1
G0Z0
M212
C0
M205
M202
M30

You do have to lock and unlock the spindle between rotations otherwise it will try to index C with the brake on and throw a servo alarm.

Mazatrol had M248 before every feed but it seem like as long as you call it on the first feed, it works.

Now we're trying to figure out how to C-offset to set our C0 on the setup screen. We TEACH it once we jog it to a spot, but when we go to run, it keeps indexing to machine C0. The TEACH will dump the C value into the offset but won't reset the setup C to 0. The Z-offset is working like it should.

Philabuster · Jan 12, 2023

rbmgf7 said:
We got it. Operator remembered the codes show up in the upper right hand corner of the screen when you're using Mazatrol. We can run Mazatrol just can't program until we get some training (trying to break these people free from being button pushers).

Seems the solution is M248 which I found to be called "spindle speed check for interlocking the start of cutting".

So our simple program that finally ran is:

T0101
G0Z0C0
G98M203S2000
M210
M248
G1Z-1F10
G0Z0
M212
C180
M210
G1Z-1
G0Z0
M212
C0
M205
M202
M30

You do have to lock and unlock the spindle between rotations otherwise it will try to index C with the brake on and throw a servo alarm.

Mazatrol had M248 before every feed but it seem like as long as you call it on the first feed, it works.

Now we're trying to figure out how to C-offset to set our C0 on the setup screen. We TEACH it once we jog it to a spot, but when we go to run, it keeps indexing to machine C0. The TEACH will dump the C value into the offset but won't reset the setup C to 0. The Z-offset is working like it should.

Are you just drilling holes and or milling slots? What features are you trying to machine?

rbmgf7 · Jan 12, 2023

Philabuster said:
Are you just drilling holes and or milling slots? What features are you trying to machine?

Just poke some holes for the time being. If we can figure out the mill, that may come in helpful but we don't have a Y axis.

Philabuster · Jan 12, 2023

rbmgf7 said:
Just poke some holes for the time being. If we can figure out the mill, that may come in helpful but we don't have a Y axis.

I don't have a Y-axis either. My machine is one generation older than yours.
Here's a video showing how to drill and tap on the face of the part with the C-axis.

rbmgf7 · Jan 12, 2023

Philabuster said:
I don't have a Y-axis either. My machine is one generation older than yours.
Here's a video showing how to drill and tap on the face of the part with the C-axis.

Appreciate it. Got a Patreon? Wouldn't mind chipping in some beer money.

So we mostly machine cast parts that'll have 3 or 4 lobes that get drilled so we need to teach a C0. I skimmed a couple videos but didn't see where I can set the C-offset for Gcode.

Mazatrol T32-3 EIA programming codes for live tooling and C axis

Aluminum

Plastic

Aluminum

Aluminum

Cast Iron

Aluminum

Cast Iron

Aluminum

Cast Iron

Aluminum

Aluminum

Diamond

Aluminum

Aluminum

Cast Iron

Aluminum

Diamond

Aluminum

Diamond

Aluminum

Similar threads