[TomFerret]

Hey all.... I have been lurking here for quite sometime. I have found out some great information from everyone here.

But the time has come that I finally cant figure something out.

I am trying to set up and run a YAM CK2 with a Fanuc 6T-B control. I think its like version 05

I have figured out how to set the tool offsets. But when I go into a program and run an offset, the control shows the difference between the programmed dimension and the offset

IE:
T0202 G0 X1. Z1. (if the offset in X is +.4 and the in Z +.4 it reads like this: X1.4 Z1.4)

I have never had this happen to me before. It is in my limited understanding that when looking at the screen it should always show the programmed dimension, as programmed.

Another issue is this... it seems this machine does EVERYTHING in incremental positions.

Any help would be GREATLY appreciated.

Thanks a million
Tom

[tc429]

there is a bit parameter that says position display includes offset or not, cant recall where, but its like in the first 30 IIRC... just flip thru the first few parameter setting pages in the maintenance book, its there


on the abs/inc thing- you might be used to newer T controls where U/W are incremental moves of X/Z axes, and programmed X/Z are absolute...in the older ones, G90 and G91 are modal, G90 selects absolute, G91 incremental... if using g28 or g30 dont forget your g91- if you call g28 z0 in absolute(g90) mode, it goes to zero then home- usually thats a very bad thing g91g28z0 just goes straight to home...

if youre used to newer Gcode system, might want to look over the gcode list and be sure its compatible with what youre running...aside from G91 vs U/W, the only other obvious thing might be G92 instead of G50 for coord presets- some of the older 6Ts wont support geometry offsets without a firmware update so theyll accept the option. using G92 sucks as its too easy to crash.

[fordav11]

we had a Mazak Powermaster with 6T many years ago. on the panel there was a switch "Manual Absolute"
If it's not ON the machine moves in incremental. If your machine has such a switch check it.
6T will accept U and W without anything extra. You don't need to switch the mode Absolute/Incremental using a G code.
No 6T's have geometry offsets as far as I know. You have to set each tool with G50 usually on a lathe and G92 on a mill.
I don't know when geometry offsets were added but I've seen them on 10-series controls but never on 6-series.

[TomFerret]

Hey Guys,

Thanks for the responses. I think that I may have to figure out where or what parameter to enable/disable.

I have looked for a Manual Absolute switch on the control panel. There is none that I can find. I looked for that first because I used to run a Wassino with an O controller.

I have also found that you have to type G50 for every offset, as well you have to have a safe program start point. This machine physically moves to compensate for the offset (if you don't program a move to a program start position).

From what else I have found you can use U and W. ie: G28 U0W0 will send it home.

We have also tried G90 in MDI. When this is done the machine alarms out. But if a G90 is in the safety call for the program it accepts it, but doesnt change the actual readout on the control. ie: G20 G40 G90

I will try the G92. I am running a Schiess/Froriep VTL built in 1984 that requires a G92.

The only thing I have left out is this.... Apparently up until about a month ago the machine ran and read out perfectly fine. I have gone over the programs that have been run on it. They are all standard G-code with no strange variances. But... the owner had a person running the machine and this person said that all he had done was type in G00 U-- W-- (not sure what numbers he put in). After doing that the display screen no longer showed the programmed dimension, but started to show the programmed dimension + the offset. Also, just a days after that a transformer in the machine cooked and had to be replace.

Not sure if any of this help... but again thanks a million guys

[angelw]

Hey Guys,

Thanks for the responses. I think that I may have to figure out where or what parameter to enable/disable.

I have looked for a Manual Absolute switch on the control panel. There is none that I can find. I looked for that first because I used to run a Wassino with an O controller.

I have also found that you have to type G50 for every offset, as well you have to have a safe program start point. This machine physically moves to compensate for the offset (if you don't program a move to a program start position).

From what else I have found you can use U and W. ie: G28 U0W0 will send it home.

We have also tried G90 in MDI. When this is done the machine alarms out. But if a G90 is in the safety call for the program it accepts it, but doesnt change the actual readout on the control. ie: G20 G40 G90

I will try the G92. I am running a Schiess/Froriep VTL built in 1984 that requires a G92.

The only thing I have left out is this.... Apparently up until about a month ago the machine ran and read out perfectly fine. I have gone over the programs that have been run on it. They are all standard G-code with no strange variances. But... the owner had a person running the machine and this person said that all he had done was type in G00 U-- W-- (not sure what numbers he put in). After doing that the display screen no longer showed the programmed dimension, but started to show the programmed dimension + the offset. Also, just a days after that a transformer in the machine cooked and had to be replace.

Not sure if any of this help... but again thanks a million guys

It will be unlikely that your control will use G92, particularly if it digests U, W and G50. G92 is the the coordinate setting G code used mainly with machining center controls and corresponds to G50 used in lathe controls.

As ford stated, no 6T controls had geometry offsets. Coordinate System set via work shift was introduced for the first time in 6MB controls.

Typically, using a 6T control, the coordinate system is set for each tool by programming G50 in association with X and Z. The values of X and Z correspond to distance from the current tool location (usually the tool change position) to the X Z zero of the workpiece. The position where the G50 is commanded should be one that is easily obtained and repeated, ie, the Zero Return for X and Z, or an incremental distance away from Zero Return.

I'm not sure how you are setting your coordinate system, particularly with your comment "you have to type G50 for every offset". Accordingly, following is one method of obtaining the G50 for each tool in X and Z.

1. With the workpiece mounted in the chuck, or work holding device, manually cut a diameter and without moving the tool in the X axis, measure and via MDI, command G50 X (and the measured diameter value). This will set the X position display to the current X position value.

2. If the end of the workpiece farthest from the chuck is Z Zero, take a light cut on the end of the work and without moving the tool in the Z axis, determine via measurement, how much material is left between the tool and Z Zero. Set the Z position display in the same manner as for X in point 1.

3. Perform Zero Return for each axis. The displayed values after Zero Return has been completed are the X and Z G50 values.

4. Its common to use the Integer component of the value obtained in 3 as the G50 and the decimal component in the tool offset. Its unlikely that the Real Number value will be exactly the same each time you subsequently set the program. Using the Integer part of the coordinate give consistency in the part program, with any variation being accommodated in the tool offset.

5. If the machine has large X and Z travels, short G50 positions can be conveniently obtained by performing a Zero Return, as in 3, and then shift the slides a whole number incremental amount closer to the workpiece. The shift position is therefore a predictable location and its X Z display values become the G50 or each axis. In the part program, an Automatic Zero Return and the incremental shift commands for each tool can be put in block delete, so that the G50 position can be easily obtained if required due to cutting tool insert change, or for whatever reason the program is stopped with the tool out of position.

Regards,

Bill

[TomFerret]

When I said that I have to apply G50 for every offset this is what I meant:
G20 G40 G90
T0100
G50 T0101 G0 X1. Z1. (movement from safe point to part)
Sorry for being unclear about that.

When I set G50 for T0100 and then home the machine (G28 U0W0) the display will be say X11.515 Z10.613. For consistency and ease I will use X11.51 Z10.61.
If I activate the offset for T0200 (T0202 with X being .4 and Z.4) and send the tool a safe position (X1. Z1.) it will go where I want it to but the display reads X1.4 Z1.4. It should be reading X1. Z1.

If from this point I send the tool home (G28 U0W0) the home position with or without cancelling the offset it display the difference of the offset at the home position. So this tells me that the machine is moving only in incremental positions.

Unfortunately I dont have a manual with the bit parameters for this machine and I am trying to get a hold of one now. For all that I can see on the both control panels there is no Manual Absolute switch.

And that brings me to the next strange thing about this machine. It has two separate control panels. Many of the switches are the same on both. But one has the CRT screen and Fanuc keyboard. This is where you load, edit etc with the programs. The second control has the Cycle Start, Stop and Feed and Rapid overrides. As well the second panel controls the tailstock.

I have run a few machines with separate controls for the tailstock but none quite like this. From the main control you cannot start, stop, turn on/off coolant, etc.

I can run this machine like this quite easily, but I cannot put a less experiences operator on it. They may get confused by the display, or worse yet end up crashing the machine.

Thanks again, and sorry for being a pest about this, but I really need to get this machine going.

Tom

[angelw]

When I said that I have to apply G50 for every offset this is what I meant:
G20 G40 G90
T0100
G50 T0101 G0 X1. Z1. (movement from safe point to part)
Sorry for being unclear about that.

When I set G50 for T0100 and then home the machine (G28 U0W0) the display will be say X11.515 Z10.613. For consistency and ease I will use X11.51 Z10.61.
If I activate the offset for T0200 (T0202 with X being .4 and Z.4) and send the tool a safe position (X1. Z1.) it will go where I want it to but the display reads X1.4 Z1.4. It should be reading X1. Z1.

If from this point I send the tool home (G28 U0W0) the home position with or without cancelling the offset it display the difference of the offset at the home position. So this tells me that the machine is moving only in incremental positions.

Unfortunately I dont have a manual with the bit parameters for this machine and I am trying to get a hold of one now. For all that I can see on the both control panels there is no Manual Absolute switch.

And that brings me to the next strange thing about this machine. It has two separate control panels. Many of the switches are the same on both. But one has the CRT screen and Fanuc keyboard. This is where you load, edit etc with the programs. The second control has the Cycle Start, Stop and Feed and Rapid overrides. As well the second panel controls the tailstock.

I have run a few machines with separate controls for the tailstock but none quite like this. From the main control you cannot start, stop, turn on/off coolant, etc.

I can run this machine like this quite easily, but I cannot put a less experiences operator on it. They may get confused by the display, or worse yet end up crashing the machine.

Thanks again, and sorry for being a pest about this, but I really need to get this machine going.

Tom

Hi Tom,

Setting the coordinate system in the way your example shows is not a good method, and may be the reason you believe that the control is moving incrementally in some way.

About the only the only thing I like about your program snippet is that you're calling the tool offset on a move line. Calling the tool offset at the same time the tool is initially called normally results in a move equal to the offset whilst the tool is indexing into place. By calling the offset during a move results in a seamless application of the offset.

When using the machine set to metric, as is most frequently used in Australia, using the integer part of the actual G50 coordinate as the G50 and the decimal component as the offset, will always result in an offset less than 1.0mm (approx 0.040inches); thus a small offset and a nice round, consistent G50. Next time the machine is set up to run the same program, its unlikely that the G50 will be more than 1mm out (approx 0.040inches); accordingly, the G50 in the program will be still correct. I round down to obtain the G50 value to be written in the program for two reasons:
1. No calculations are required, you simply take the decimal component as read.
2. The offset will be stored as a negative value offset. On most machine tools, if the offset was called when the slides were at Zero Return and not on a move line, then the slides will be offset away from the Zero Return position, with no chance of the slides going into over travel.

When using the machine set to Imperial input, if the above method were to be followed, the tool offset could be up to 0.9999; I would avoid using a tool offset that large on a Series 6T control. In the case of Imperial input, I round down to the closest 0.1inch, resulting in the initial offset being no larger than 0.0999 (approximately 2.5mm). Accordingly, using your example, the G50 in the program would be G50 X11.5000 Z10.6000, with offsets of -0.015 and -0.013 for X and Z respectively.

The preferred method of setting the coordinate system via G50 is as follows, and should be done with the slides at a known, repeatable position.
(Example actual G50 = X11.515 Z10.613)
(X Z offset = -0.015 and -0.013 respectively)
N1 G20 G40 G90
G28 U0.0 Z0.0
G50 X11.5000 Z10.6000
G50 T0100 S3000
G96 S600 M03
G00 X1.0 Z0.5 T0101 M08
...........
...........
...........
...........
...........
...........
G28 U0.0 W0.0 T0100 M09
M01
(Example actual G50 = X10.426 Z11.752)
(X Z offset = -0.026 and -0.052 respectively)
(TOOL CHANGE)
N2 G28 U0.0 Z0.0
G50 X10.4000 Z11.7000
G50 T0200 S3000
G96 S600 M03
G00 X1.0 Z0.5 T0202 M08
...........
...........
...........
...........
...........
...........
G28 U0.0 W0.0 T0200 M09
M01

etc

Its important that the G50 be commanded with the tool offset canceled, hence the reason in the above example of canceling the tool offset on the move line back to the tool change position. If this is not done, there will be a gradual shift of the G50 equal to the offset amount. This shift will be accumulative if not going back to the Zero Return location before commanding the next G50.

Give the above format a try and see if the machine is still moving incrementally as you say. I'd be surprised if it does.

Regards,

Bill

[Lyfordln1]

I have an Ikegai with 6T control and I program this way:
G28W0
G28U0
G00W-1.0
G50X00
Moo
with the machine zero returned, GO TO INCREMENTAL PAGE AND "ORIGIN" X & Z
TOUCH OFF THE FACE AND OD AND ENTER THE MEASUREMENT IN YOUR OFFSET. ON THE ON, ENTER DISTANCE FROM HOME, THEN "U-DIAMETER MEASURED.
N1T0100
G0G97S100M8
X1.0Z.05T0101M3

AT END OF THIS TOO
G00X0Z0T0100
M01
AFTER SETTING YOUR OFFSETS, i JUST GO DOWN WITH THE 1ST TOO WITH OFFSET ACTIVATED AND SEE WHAT THE DIFFERENCE FROM LAST JOB AND CHANGE THE GO W-1.0 NEAR BEGINNING OF PROGRAM TO ALLOW FOR THE DIFFERENCE. THIS WAY YOUR OFFSETS REMAIN THE SAME JOB TO JOB.

[TomFerret]

Hi Tom,

The preferred method of setting the coordinate system via G50 is as follows, and should be done with the slides at a known, repeatable position.
(Example actual G50 = X11.515 Z10.613)
(X Z offset = -0.015 and -0.013 respectively)
N1 G20 G40 G90
G28 U0.0 Z0.0
G50 X11.5000 Z10.6000
G50 T0100 S3000
G96 S600 M03
G00 X1.0 Z0.5 T0101 M08
...........
...........
...........
...........
...........
...........
G28 U0.0 W0.0 T0100 M09
M01
(Example actual G50 = X10.426 Z11.752)
(X Z offset = -0.026 and -0.052 respectively)
(TOOL CHANGE)
N2 G28 U0.0 Z0.0
G50 X10.4000 Z11.7000
G50 T0200 S3000
G96 S600 M03
G00 X1.0 Z0.5 T0202 M08
...........
...........
...........
...........
...........
...........
G28 U0.0 W0.0 T0200 M09
M01

etc

Its important that the G50 be commanded with the tool offset canceled, hence the reason in the above example of canceling the tool offset on the move line back to the tool change position. If this is not done, there will be a gradual shift of the G50 equal to the offset amount. This shift will be accumulative if not going back to the Zero Return location before commanding the next G50.

Give the above format a try and see if the machine is still moving incrementally as you say. I'd be surprised if it does.

Regards,

Bill

Thanks a million for all of the help. I have done exactly as you said. plus a few variations. The machine is still reading in incremental.

We were able to find the bit parameter that needed to be changed to supposedly have the control display absolute. But that still didnt work.

I am really at my wits end with this control. As far as I can tell there is no manual absolute switch. I will post a couple of pics of the control tomorrow. But i am pretty certain because we found a list of the switches on the control.

Any more help would be greatly appreciated.

[angelw]

Thanks a million for all of the help. I have done exactly as you said. plus a few variations. The machine is still reading in incremental.

Hi Tom,
Just to ensure that we are both on the same page, are you saying that in the following code, when the block highlighted in RED is executed, the X and Z slides move 0.5" (X1.0 diameter / 2) and 0.5" respectively in a plus direction away from the work, rather than to a diameter of 1.0" and 0.5" from the Z Zero of the work?

Also, do the following test.

1. Park the slides well away from the chuck and any thing else it may be able to hit, and well away from the over travel area of the machine.
2. Input the following program and execute.

N1 G00 G20 G40 G94
G50 X2.0 Z2.0
G00 X3.0 Z3.0 (INCREMENTALLY THE SLIDES WILL MOVE A DISTANCE OF X3.0 (DIAMETER) AND Z3.0)
-----------------(ABSOLUTE THE SLIDES WILL MOVE A DISTANCE OF X1.0 (DIAMETER) AND Z1.0)
G01 X-1.0 Z-1.0 F1000 (INCREMENTALLY THE SLIDES WILL MOVE A DISTANCE OF X-1.0 (DIAMETER) AND Z-1.0)
---------------------------(ABSOLUTE THE SLIDES WILL MOVE A DISTANCE OF X-4.0 (DIAMETER) AND Z-4.0)
M30

3. What happened?


Regards,

Bill

N1 G20 G40 G90
G28 U0.0 Z0.0
G50 X11.5000 Z10.6000
G50 T0100 S3000
G96 S600 M03
G00 X1.0 Z0.5 T0101 M08

[TomFerret]

Okay.... so the machine is moving in absolute. So i feel like a bit of putz.

I think that I have confused myself in that respect. But the core issue still remains.

The display still shows the offset added to the programmed diameter and length.

It should read X1.0 Z.5. If the offset in T0101 is X.035 Z.035 the display shows X1.035 Z.535.

I have looked for a bit parameter in regards to just the display and havent been able to find one.

[fordav11]

there is a parameter for that for sure. I know because I changed it on my control back when I worked a 6-series many, many years ago.

[oldgoat]

OK, I'm not sure if this is what you are looking for, it has been at least 15 years since I touched a 6T control.

Parameter 010.2 [PROD]

1: Position programmed in present value display is displayed.
0: Actual cutter position with tool position offset and tool nose radius compensation is displayed.

Taken from a GN6T Series B Operator's Manual. Deciphering of the actual meaning of the translation is left to you. Use at your own risk...

Ken

[fordav11]

yeah that's the one. it should be set to 1 and the display will show only the program positions.

[TomFerret]

OK, I'm not sure if this is what you are looking for, it has been at least 15 years since I touched a 6T control.

Parameter 010.2 [PROD]

1: Position programmed in present value display is displayed.
0: Actual cutter position with tool position offset and tool nose radius compensation is displayed.

Taken from a GN6T Series B Operator's Manual. Deciphering of the actual meaning of the translation is left to you. Use at your own risk...

Ken

Hey Ken thanks a million. I am going to hunt this down and give it a try. The worst that will happen is that I have to put the parameter back to what it was originally.

Will let you guys know in a couple of days what happened.