Hi everyone.
I have been using fanuc controlers but am now using a mazak nexus 350.
In adition to the mazak programming im also trying to continue using gcode iso programming when i feel the need.

I have tried to write a g71 cycle in the format that i used to write on the funuc control but i am getting an error when i put radius compensation in the cycle.

On the fanuc i used to write like this:

G21 G50 S3000
G28 U0 W0
T0101 G40 G99 G96 S200 M04
G00 X40 Z1
G71 U2 R1
G71 P10 Q20 U.3 W.05 F.25
N10 GOO G42 X0
G01 Z0
X20
Z-10
X35
Z-30
X40
N20 G40
G28 U0 W0
M01
G28 U0 W0
T0202 G40 G99 G96 S250 M04
G00 X40 Z1
G70 P10 Q20 F.05
G28 U0 W0
M30

Thats how i used to write, but when i try that on the mazak it doesnt like the g42. i know that the fanuc used to ignore the g42 in the roughing cycle but then in the finishing cycle it would pick it up .

Can anyone shed some light on the whole g42 g41 situation and how the machine uses it.
Maybe the compensation is always on? or do i need to specify it on each tool or what?

Thanks for your help in advance

Cheers

What is the error you are getting?

- What is the control ? 640 T or Matrix ?
- Do you think to set the correct P value in EIA tool offset ( P1 to P9 ) ?
- Do you work with EIA offset or "Mazatrol" Tool data ?

Hi Steelcutter and Froggy, thanks very much for the responses.
The error i get is 898 lap cycle illegal shape design.
The control is mazatrol matrix. the one with the very irritating safety shield and even more irritating voice thingy that says something everytime i touch the control.

Froggy i think you are on to something, let me explain my situation: I have started working for a new company and they use mazak, its not difficult work and it does not require the precision im used to in formula one , aerospace etc.
So the guy i replaced was not really learning much on the machine and so now im learning the mazak control on my own with not much help from anyone as they know nothing. I have been using the normal mazak programming for the last 3 weeks but i have to say i prefer my old method of gcode fanuc style.

So the last two days i have been trying to write gcode as i used to but i suspect as you pointed out i have made a few mistakes and am getting mixed up with the two formats the machine uses ie mazak and eia/iso.

So please could you help me, maybe just a step by step quick guide on what, how i should set my tool data etc.

Froggy i think you are right as i have touched all my tools on on the tool eye and entered the data the same way as i was shown for mazak program , ie i enter data on the TOOL DATA page and it shows pictures and stuff and i choose between inside or outside tool, groove tool bla bla bla etc.
So maybe my iso program is not picking up on that info?

On the fanuc for a normal turning tool i used to set the x offset z offset and then enter the tool nose radius and then enter the tool position ( position 3 in my case) I used to enter it all on one line on the tool offset page of the fanuc control.

Is there a way for me to set my tools like this on the mazak?

Guys i really appreciate the responses , so thank you very much for your time.

Any information you can give me on this machine when it comes to g code would really help.

Cheers.

So is there a separate page for setting my tool data for iso program?
I will have a good look tomorrow when i get to work and see if i can find something.

Thanks guys

The most profound thing we need to know is the control type - Fusion or Matrix?

Fusion has parameters P9 and P16. This determines "T32 compatible" G code Type A, B or C, or "Standard" G code type A, B or C.

This A, B or C covers G code standard for lathes from I would guess about 1978 to 1990 or so. The charts for this are in the EIA programming manual. G94, G95, G99 and G99 and G12.1 are where most of the difference lies, but also in the format for Fanuc type G70 through G76.

For the Matrix, the g code type is fixed to the most modern version of G code standards for cnc lathes and does not allow parameterization for obsolete and hybred G codes.

The next issue is the G code T word - can be four or six digits, by parameter. This is covered in the T word section of the EIA manual and specs the parameter needed to switch 4 to 6 and vice versa.

For 4 digit T word, the format is TAABB. AA is the turret station, BB is if you want to attache the EIA offset registers to your tool. I prefer using the "mazatrol coordinate system", which is usually G53.5, or just G53.

The beauty of the mazatrol coordinate system is that it uses the Z offset of your set up page (important concept - there is a set up page for each program, regardless of mazatrol or G code) and the tool set in Mazatrol Tool Data. The major benefit to mazatrol coordinates is that the Z offset remains in effect CONSTANTLY, and the TOOL OFFSET does the same. In other word, Z offset is by virtue of the active program, and Tool offset is by virtue of turret index. Neither can be extinguished by reset!

This allows you to use the wonderful teach function of mazatrol operation and also allows you to take tool set values right off the tool eye. the tool set can also be done manually for both axes, but the Z value is with respect to machine Z zero datum, not the Z offset value. An incremental correction by the Z offset value associated with the part you're touching off makes it absolutely correct. The main principle for tool sets with mazak are they are with respect to the machine, not the workpiece, and therefore apply to EVERY THING! This is moot in X, which is with respect to the X0 centerline of the spindle, but is helpful to understand for Z.


Hope this clears a few things up.

-90% Jimmy

if you want to use cutter comp in EIA you need to set only your quadrant and radius on the TOOL OFFSET page. And i am pretty sure you need to use the old style 1 line G71 canned cycle.

Hi everyone, thank you for all your help. Yes the issue was with me not having set my tool data in the seperate tool offset page. So now all seems to be fine. I also had issues with putting in radiuses and chamfers , even when i followed the format shown in the book. I found out that you have to put a comma, befor you write in the radius or chamfer ,c5 ,r3 . Just incase anyone gets stuck with that. Also the g71 is written in the two line format.


Once again thankyou to all of you , it really helped me to sort out my problem.

Cheers

About Voice : in diagnos screen , move the mouse near the top of the screen , click "set up", you will fing "voice adviser" with mark in front of it , click to remove the mark > Shut up !

About safety shield , try to change parameter O91 bit 7 to 0 > power off > no more safety shield ..
To access O91 you must be in "1131 mode"

diagnos > info version > right touch > 1131 > input
then diagnos > info version > new info version menu > system parameter > you get the list of O parameter

Take care : Be sure if you crash your machine in manual mode with this setting , Mazak service will laught very loud when you ask for warranty !

You can also just look for M38 and M39 parameter setting : mean distance for alamr of inteligent safety shield.

Thank you to look in your parameters book , and note value before all change to be easily able to get setting back !

Very high quality info here.

Also, please understand the Matrix has a "keystroke memory", so that if you call in Mazak service, they will be able to retrace all your keyboarding. It helps to fix problems and it also helps to get to all the history in an incident.


-90% Jimmy