[fooo]

Hi there,

I want to call a G-code program from a Mazatrol program and do some machining on the sub-spindle. The scheme looks like that:

1) Machining on the main spindle
2) Transfer workpiece
3) Machining on the sub spindle
4) Call G-code program and machining on the sub spindle

The problem I have is that the G-code program (step 4) always refers to the main spindle (i.e. it wants to do the machining on the main spindle and not the sub spindle) but the sub spindle is properly setup (step 3 proves that). How can I make it to work on the sub spindle?

Well I guess I have to do a zero-shift but how can I access the Z-OFFSET in the Setup-Page for the sub-spindle?

The control is a 640T.

Regards
Frank

[M-man]

cant it be done with a mirror image on Z-axis?

[fooo]

Hmm I don't know! What would be the G-code for this?

[arie2003]

what did you do on step 3?
secondary/sub spindle have different M code with main spindle.
did you try to put M300 (secondary spindle selection) on the top of second spindle program?
another M code for secondary spindle :
M303 normal rotation
M304 reverse rotation
etc
please refer to M code list on operating manual book

[fooo]

Well I can make the sub spindle turn and I think I put M300 at the beginning of the program but lets say if I put in G00 Z0 it moves toward the main spindle and not toward the sub spindle so it looks like to me that there is an issue with the zero point.

In the Setup-Page there's a Z-Offset data item for each transfer that tells the control to shift the zero point so machining can be done on the subspindle after the transfer is completed. It looks like to me this offset is not considerated when I call the ISO sub program.

[chucker]

Just wondering can you use your g54 through g59 work offsets to set a new zero point at the face of your part in the sub spindle then program Z in the + direction.

[fooo]

Sure I can setup and use one of those zero points but I find it awkward to do and I thought the Mazatrol coordinatesystem takes care of it automatically...

[slavetothemetal]

What about tool control? I am not a Mazak guy, but do you need to specify anything differently for the tool offset?

[Lathejockeu81]

On the 640MT Pro Integrex, this is controlled by a parameter. One way all EIA subs refer to the main spindle WPC... the other way it uses whatever WPC is correct for the active spindle.

There also may be a parameter to use independent WPCs... using the setup page for the EIA sub to set it and activating the "Mazatrol" WPC with a G53.5P2 in the sub program... obviously not best way, but it might be an option.

Also... settting the WPC manually should not be difficult. Take the absolute value of the transfer point and add the Z offset for the main spindle. This is the point of the rightmost face of the part on the subspindle. We have to set the Z2 offset manually when we run straight EIA and setting Z offsets and transfer points has never been a problem.

[fooo]

On the 640MT Pro Integrex, this is controlled by a parameter. One way all EIA subs refer to the main spindle WPC... the other way it uses whatever WPC is correct for the active spindle.

Thanks for your reply. I looked for that paramter you describe here but couldn't find it. Any chance you can figure out what it was?

Regards
Frank

[crazythunder]

Well on our Integrex with the 640Mt PRO control there is not a parameter for using the sub spindle. You just call up the W axis and that will move it to the correct position if you are wanting to use it to pick parts from the main spindle.

Here is a sample code set for swapping parts from one spindle to the next I got from a friend:
M307
M202M302G10.9X1
G20G80G40G17G90G94G98
G91G53G0X0.
G91G28X0.
T2.1M6
G91G53G0X0.
G91G28X0.
M107
G91G28Y0.
G91G28Z0.
G91G28W0.
(HEAD I JAW WASH)
G97M203S100R1
G90G53Z6.0B0.
M107
G53X-41.22
G94G4X5.M51M8
M205M9
(HEAD II JAW WASH)
G91G28X0
G90G53Z14.5B180.
M107
G97M303S100R2
G53X-41.22
G94G4X5.M51M8
M305M9
G91G28X0.
G91G28Y0.
G91G28Z0.B0.
M107
M0
#600=-48.353
G17G40G80G90G94G98
G94M540M306(M540 TRANSFER MODE ON)
G4X2.
M200M300
G0C0.U0.
M210M310
M508
G90(TRANSFER PUSH)
G0W[#600+.7]
G1W[#600+.6]F3.9
G91G1G31W-.678F3.9
#601=#5026
#5243=[#5223+ABS[#600]Z(WRITE TO G55 Z WORK OFFSET)
IF=[#601GT#600]GOTO5000
G55
G4X2.
M307
G4X15.
M206
G4X15.
G91G30W0
M541(M541 TRANSFER MODE OFF)
M212M312
M99
N5000
#3000<50(HEAD_II_XFER_MISPOSITION)

I hope that gives you some ideas and help

[Lathejockeu81]

I was not referring to part transfer. I was referring to the use of an EIA sub to do work on the sub spindle AFTER a transfer was performed in Mazatrol. Unfortunately I'm at home so I don't have the parameter list handy... but it's definately there.

However I must say that I've not seen a transfer routine with dynamic Z2 offset correction and error checking before. Very nice.

I also noticed that your transfer feedrate is 3.9ipm. Were you experiencing false reads in your transfers at higher feedrates? I would like to know because our incredibly effective Mazak service center doesn't know how to decrease the sensitivity during W axis skip feeding... Perhaps we are not the only ones with this problem?