problems running g code (EIA/ISO) on a mazak quick turn 15 with a cam t2 controls

hello,I have a mazak quick turn 15 with a cam t2 control that were able to load a program on,but when we go to run it, it homes,a clicking sound as if it were to start happens but it doesn't move or alarm out?it also runs mazatrol fine so we know the machine works.we tried multiple post using iso and eia but they all only get to the clicking sound which im guessing is to start the spindle.Could it be a parameter or the post or somthing else were doing wrong?any help would be great,thanks

Could you take a picture of the program?

O0100 ( IT001474-32 )


(HOLE1 DRILL ID_20000_2:TN )
N4 G50 X10.0 Z5.0 S400 M43
N5 G00 T0707
N6 G97 S400 M04
N7 G00 X-0. Z0.1181 M8
N8 G01 Z-2.0 F0.02
N9 Z0.1181
N10 Z-1.8819
N11 G01 Z-3.0744
N12 Z0.1181
N13 M05
N14 M09
N15 G28 U0 W0
N16 G00 T0700
N17 M01

( BORE1 ROUGH BORE WN_B_Small_80_RH)
N19 G50 X10.0 Z5.0 S593 M43
N20 G00 T1313
N21 G97 S593 M04
N22 G00 X-2.0497 Z0.1181 M8
N23 Z0.1045
N24 G01 Z-3.0005 F0.008
N25 X-2.0
N26 X-1.9722 Z-2.9866
N27 Z0.1045
N28 G01 X-2.0994
N29 Z-3.0005
N30 X-2.0497
N31 X-2.0219 Z-2.9866
N32 Z0.1045
N33 G01 X-2.1492
N34 Z-3.0005
N35 X-2.0994
N36 X-2.0716 Z-2.9866
N37 Z0.1045
N38 G01 X-2.1989
N39 Z-3.0005
N40 X-2.1492
N41 X-2.1213 Z-2.9866
N42 Z0.1045
N43 G01 X-2.2486
N44 Z-3.0005
N45 X-2.1989
N46 X-2.171 Z-2.9866
N47 Z0.1045
N48 G01 X-2.2983
N49 Z-3.0005
N50 X-2.2486
N51 X-2.2208 Z-2.9866
N52 Z0.1045
N53 G01 X-2.348
N54 Z-3.0005
N55 X-2.2983
N56 X-2.2705 Z-2.9866
N57 Z0.1045
N58 G01 X-2.3978
N59 Z-3.0005
N60 X-2.348
N61 X-2.3202 Z-2.9866
N62 Z0.1045
N63 G01 X-2.4475
N64 Z-3.0005
N65 X-2.3978
N66 X-2.3699 Z-2.9866
N67 Z0.1045
N68 G01 X-2.4972
N69 Z-3.0005
N70 X-2.4475
N71 X-2.4196 Z-2.9866
N72 Z0.1045
N73 G01 X-2.5469
N74 Z-3.0005
N75 X-2.4972
N76 X-2.4694 Z-2.9866
N77 Z0.1045
N78 G01 X-2.5966
N79 Z-3.0005
N80 X-2.5469
N81 X-2.5191 Z-2.9866
N82 Z0.1045
N83 G01 X-2.6464
N84 Z-3.0005
N85 X-2.5966
N86 X-2.5688 Z-2.9866
N87 Z0.1045
N88 G01 X-2.6961
N89 Z-3.0005
N90 X-2.6464
N91 X-2.6185 Z-2.9866
N92 Z0.1045
N93 G01 X-2.7458
N94 Z-3.0005
N95 X-2.6961
N96 X-2.6682 Z-2.9866
N97 Z0.1045
N98 G01 X-2.7955
N99 Z-3.0005
N100 X-2.7458
N101 X-2.718 Z-2.9866
N102 Z0.1045
N103 G01 X-2.8452
N104 Z-3.0005
N105 X-2.7955
N106 X-2.7677 Z-2.9866
N107 Z0.1045
N108 G01 X-2.895
N109 Z-3.0005
N110 X-2.8452
N111 X-2.8174 Z-2.9866
N112 Z0.1045
N113 G01 X-2.9447
N114 Z-3.0005
N115 X-2.895
N116 X-2.8671 Z-2.9866
N117 Z0.1045
N118 G01 X-2.9944
N119 Z-3.0005
N120 X-2.9447
N121 X-2.9168 Z-2.9866
N122 Z0.1045
N123 G01 X-3.0441
N124 Z-3.0005
N125 X-2.9944
N126 X-2.9666 Z-2.9866
N127 Z0.1045
N128 G01 X-3.09
N129 Z-0.1346
N130 X-3.0535 Z-0.1662
N131 G02 X-3.0441 Z-0.1838 I0.0305 K-0.0176
N132 G01 X-3.0163 Z-0.1698
N133 Z0.1045
N134 G01 X-3.1358
N135 Z-0.0949
N136 X-3.09 Z-0.1346
N137 X-3.0621 Z-0.1207
N138 Z0.1045
N139 G01 X-3.1816
N140 Z-0.0552
N141 X-3.1358 Z-0.0949
N142 X-3.108 Z-0.081
N143 Z0.1045
N144 G01 X-3.2275
N145 Z-0.0155
N146 X-3.1816 Z-0.0552
N147 X-3.1538 Z-0.0413
N148 Z-0.0155
N149 G01 X-3.2275
N150 X-3.1996 Z-0.0016
N151 X-2.8079
N152 Z-0.1838
N153 G01 X-3.0441
N154 G02 X-3.0444 Z-0.1868 I0.0352 K0.
N155 G01 X-3.09 Z-0.4473
N156 Z-3.0005
N157 X-3.0441
N158 X-3.0163 Z-2.9866
N159 Z-0.4473
N160 G01 X-3.09
N161 X-3.1358 Z-0.7093
N162 Z-3.0005
N163 X-3.09
N164 X-3.0621 Z-2.9866
N165 Z-0.7093
N166 G01 X-3.1358
N167 X-3.1816 Z-0.9712
N168 Z-3.0005
N169 X-3.1358
N170 X-3.108 Z-2.9866
N171 Z-0.9712
N172 G01 X-3.1816
N173 X-3.2275 Z-1.2332
N174 Z-3.0005
N175 X-3.1816
N176 X-3.1538 Z-2.9866
N177 Z-1.2332
N178 G01 X-3.2275
N179 X-3.2733 Z-1.4952
N180 Z-3.0005
N181 X-3.2275
N182 X-3.1996 Z-2.9866
N183 Z-1.4952
N184 G01 X-3.2733
N185 X-3.3192 Z-1.7572
N186 Z-3.0005
N187 X-3.2733
N188 X-3.2455 Z-2.9866
N189 Z-1.7572
N190 G01 X-3.3192
N191 X-3.365 Z-2.0192
N192 Z-3.0005
N193 X-3.3192
N194 X-3.2913 Z-2.9866
N195 Z-2.0192
N196 G01 X-3.365
N197 X-3.4013 Z-2.2264
N198 Z-2.3325
N199 G03 X-3.3865 Z-2.3499 I-0.0242 K0.
N200 G02 X-3.365 Z-2.3752 I0.0244 K-0.0253
N201 G01 X-3.3372 Z-2.3613
N202 Z-2.2264
N203 G01 X-3.4013
N204 Z-2.3325
N205 X-3.3734 Z-2.3186
N206 X-2.8179
( FINISH BORE1 )
N208 G50 S783
N209 G97 S783 M04
N210 G00 X-2.8179 Z0.1137 M8
N211 X-3.3879
N212 G01 X-3.0625 Z-0.1681 F0.004
N213 G02 X-3.0541 Z-0.1838 I0.0271 K-0.0156 F0.0012
N214 X-3.0543 Z-0.1865 I0.0313 K0.
N215 G01 X-3.4113 Z-2.2262 F0.004
N216 Z-2.3325
N217 G03 X-3.3941 Z-2.3528 I-0.0282 K0. F0.0012
N218 G02 X-3.375 Z-2.3752 I0.0217 K-0.0225
N219 G01 Z-3.0005 F0.004
N220 X-3.1638 Z-2.8949
N221 X-2.8179
N222 Z0.1181
N223 M05
N224 M09
N225 G28 U0 W0
N226 T1300
N227 M30


we tried a couple different ways including taking the numbers out and rewriting the heading but still nothing,could it be the parameters are not set right to run eia? thanks for the help.

Boy I guess I am spoiled already I can't imagine writing all that compared to mazatrol. My machine has eia but I don't intend to use it, other than some manual processes in mazatrol, unless i get a job for a million parts or so and need to really optimize to the max. Sounds like you don't have a clue where the problem is. Personally if I was in that state I would start with a little bitty program to maybe start off with just facing the part and build from there.

I don't think cam t2 can run eia/iso programs at all.

theres another 4 line program that mazak sent but it just homes and moves an inch then rehomes. I think it may be in the way we're telling it to start the spindle scince it usually only gets to the 3rd line in the program But I'm not entirely sure?

I'm not sure either but it does have parameters asking to set eia/iso and the program does go in and load and it starts it just won't get past the 3rd or 4th line.

whats M43 ?

The manual states(external command of mcode 3)
from what I see reading it again it contradicts the m04 that were trying to turn it in, so I'm gonna change that and see what we're at from there, thanks

I would take that out of your program and see if it runs.

O0100
(FACE1 FINISH FACE SW_Turn_80_RH )
N4 G50 X10.0 Z5.0
N5 G00 T0202
N6 G97 S800 M03
N7 G00 X0.95 Z0. M8
N8 G01 X-0.02 F0.006
N9 X0.1356 Z0.0778
N10 M05
N11 M09
N12 G28 U0 W0
N13 T0200
N14 M30


OK this is the code i came up with i took the m44/43 out and only did a one pass facing operation, im gonna try it on the machine and see what happens, thanks for the help guys

scraper said:

I don't think cam t2 can run eia/iso programs at all.

Click to expand...

Its an option, both my T2 and T3 has that option.

I own eia/iso programing manual for both T2 and T3.

Yes, EIA/ISO was an option on the T2 and T3.

Why run g-code on an 2 or 3 axis Mazak lathe?

3 words man: Mazatrol, Mazatrol, Mazatrol

Benganboll is there any way you could possibly send me a manual, and also on the whole mazatroll thing, at this point it's the owners decision and it was to run g code since we have haas lathes and mills and it would be eiser to move jobs between machines using Goode. Personally I like mazatroll and from what I've seen on other jobs it'll handle some complex Multi axis parts with ease and speed.

SO did this work or you still stuck?

mgutierrez64 said:

O0100
(FACE1 FINISH FACE SW_Turn_80_RH )
N4 G50 X10.0 Z5.0
N5 G00 T0202
N6 G97 S800 M03
N7 G00 X0.95 Z0. M8
N8 G01 X-0.02 F0.006
N9 X0.1356 Z0.0778
N10 M05
N11 M09
N12 G28 U0 W0
N13 T0200
N14 M30


OK this is the code i came up with i took the m44/43 out and only did a one pass facing operation, im gonna try it on the machine and see what happens, thanks for the help guys

Click to expand...

mgutierrez64 said:

Benganboll is there any way you could possibly send me a manual, and also on the whole mazatroll thing, at this point it's the owners decision and it was to run g code since we have haas lathes and mills and it would be eiser to move jobs between machines using Goode. Personally I like mazatroll and from what I've seen on other jobs it'll handle some complex Multi axis parts with ease and speed.

Click to expand...

What do you need, Both Mazatrol and eia/iso books?
Do you have any books to that machine?

I think you creates a new mazatrol program faster then taking G-codes from a haas and fine tune that suiting this machine.

If you will create mazatrol programs and want to save them, you need a software that can handle the protcol mazatrol uses.
If you dont have that I recommend http://mazview.com/ it does nothing else than saving your files and you can view them but its a good price for it (199$).

cnctoolcat said:

Why run g-code on an 2 or 3 axis Mazak lathe?
3 words man: Mazatrol, Mazatrol, Mazatrol

Click to expand...

I have one QT10N T2 and one ST30ATC m/c T3.
For the QT10N with T2 I agree 100%, dont see any point doing a eia/iso program other than in rare cases doing a manual process within mazatrol.
But my ST30ATC m/c with T3 sometimes running me crazy.
It has a 3 speed gearbox so before every process it will stall for a little time do decide what gear to use. (I think that is the reason).
I can select gear manually for the rough cut but no for the fine cuts, that is auto only, so if I have a job that only require to do the face and a small chamfer on the OD. It will then use gear 3 on the face and then stop the spindle to put in gear 2 to only do the small chamfer.

So I thinking about doing eia/iso for some parts that we do a lot of.

benganboll, I would just need the eia/iso programming manual it came with the three other books.the way we program is through featureCam
And we would only be changing post when exporting between machines not editing code.I told my boss about Mazview and he's gonna look into it, thanks for the help.

kazsub, the program that you quoted worked so know we edited the post on featurecam to get rid of the m43/44.

benganboll said:

But my ST30ATC m/c with T3 sometimes running me crazy.
It has a 3 speed gearbox so before every process it will stall for a little time do decide what gear to use. (I think that is the reason).
I can select gear manually for the rough cut but no for the fine cuts, that is auto only, so if I have a job that only require to do the face and a small chamfer on the OD. It will then use gear 3 on the face and then stop the spindle to put in gear 2 to only do the small chamfer.

So I thinking about doing eia/iso for some parts that we do a lot of.

Click to expand...

Like I said a while ago in another thread, you can edit the machine's gear change speed parameters. Lower the max speed for gear 2 down to say 500 RPM (vs 1200) and that will force machine to select 3rd gear to maintain the SFM for the finish cut.

Machine will select the lowest gear it can to maintain torque when machine gets to select the gear speed for a given process. If the max spindle programmed speed is equal or below say 1,200 RPM, machine will never choose 3rd gear on its own as 2nd gear is fast enough.

Philabuster said:

Like I said a while ago in another thread, you can edit the machine's gear change speed parameters. Lower the max speed for gear 2 down to say 500 RPM (vs 1200) and that will force machine to select 3rd gear to maintain the SFM for the finish cut.

Machine will select the lowest gear it can to maintain torque when machine gets to select the gear speed for a given process. If the max spindle programmed speed is equal or below say 1,200 RPM, machine will never choose 3rd gear on its own as 2nd gear is fast enough.

Click to expand...

Well, there is a problem with that.
The machine is using these parameters both as speed limit for each gear but also as ratio in gearbox.
So if I lower parameter GR2 from 1200 to 600 it will use gear 3 for 601->3000 RPMs but if it needs 500 rpm it will use gear 2 and thinks it 500 rpm but in real its 1000 rpm.