Fanuc G36/G37 wrong wear offset value.

[rjwalker1973]

Hello everyone,

Machine: Doosan SMX2600S
Control: Fanuc 31i-b

I use a calibrated tool (30mm ball) to set thermal parameters before using the toolsetter to set tools.
The values of the calibrated tool are known so i measure the tool with the toolsetter and adjust parameters so the wear value becomes 0.
Works great. All tools are always <0.01mm from toolsetter.

The only weird thing is that i always get a 0.07mm wear value difference between using the toolsetter manual en via G36/G37.
In my program i correct for this value so thats not a problem but i dont get why its doing that.
Speed is always 30mm/min for measuring. Its 0.07mm in X and in Z direction.

Anyone know why?

Gr

One thing did come to mind this morning. When you touch off is the manual cycle multi touch or single touch? I know most auto cycles are multi touch. That does make a slight difference.

 

[EKrol]

One thing did come to mind this morning. When you touch off is the manual cycle multi touch or single touch? I know most auto cycles are multi touch. That does make a slight difference.

Both manual and auto is single touch.

One thing did come to mind this morning. When you touch off is the manual cycle multi touch or single touch? I know most auto cycles are multi touch. That does make a slight difference.

Both are single touch. The only think i can think of is some delay with g36/g37 cause it running in auto mode vs using the toolsetter in manual mode. Or the g36/g37 is a bad macro causing delay.

 

[angelw]

Both are single touch. The only think i can think of is some delay with g36/g37 cause it running in auto mode vs using the toolsetter in manual mode. Or the g36/g37 is a bad macro causing delay.

As suggested by Sinha in his Post #19, Post a copy of the program here to get more informed help.

 

[EKrol]

I did write a little testprogram without any calculations. Just a measurement. On the G31 line it is getting stuck. The controls "distance to go" want to go up a little more but its not moving. It does not skip to the next line. If i subtract 1 mm of the X value so it does not touch the toolsetter and it will continue the program.

%
<G31TEST>

G59
(SET G59 TO ZERO)
G10L52
N1226P1R0
N1226P2R0
N1226P3R0
N1226P4R0
N1226P5R0
G11
G59

G28U0
G28V0
G28W0
M6T31031
M77(Q-SETTER-ADVANCE)
G400B-90J0
G490S0

M107(B-AXIS BRAKE RELEASE)

G53G00X502Y-105
G98
G01U-42.0F4000.0
G00W-350.0
G01W-73.0F2000.0
G01F20
G31X492.6115 <<<<
G01U-5.0
G00W100.0

G28U0
G28V0W0

N999(END)
M76(Q SETTER RETRACT)
G54
M30
%

 

[rjwalker1973]

Would lowering the percentage for your "torque" have an affect on what you are doing? ALso do you have to select the axis you are using in your g31 line? I have seen g31 used with subspindles and with probes on mills to help prevent crashes, but I'm not sure in your situation. Hopefully Bill see's this and can clarify.

 

[EKrol]

Would lowering the percentage for your "torque" have an affect on what you are doing? ALso do you have to select the axis you are using in your g31 line? I have seen g31 used with subspindles and with probes on mills to help prevent crashes, but I'm not sure in your situation. Hopefully Bill see's this and can clarify.

G31 P99 P98 is for torqueskip for takeover to subspindle. I guess G31 works on probes and on toolsetters because they are thesame right? Maybe i'm wrong here.

 

[rjwalker1973]

G31 P99 P98 is for torqueskip for takeover to subspindle. I guess G31 works on probes and on toolsetters because they are thesame right? Maybe i'm wrong here.

Not sure. Bill will know when he sees this. I am interested to know myself and Bill is tops on this stuff.

 

[angelw]

The controls "distance to go" want to go up a little more but its not moving. It does not skip to the next line. If i subtract 1 mm of the X value so it does not touch the toolsetter and it will continue the program.

What value is stored in System Variable #5061 when you execute the program with 1mm subtracted from X492.6115, it should be 491.6115? If so, the G31 function is operating correctly and I suspect that the Q Setter is not wired to the Skip Signal Input. In this case, the machine and control is operating in the same way as when manually jogging the axis onto the Q Setter, the axis travel will be halted and must be manually driven away from the Q Setter..

G31 has all the same attributes as G01 (except an alarm will be raised if G31 is issued in G41/G42 mode. Accordingly, if the axis were to be driven onto the Q Setter using G01 mode, the control would protect itself by hauling axis traverse when any of its switches are made and you would have to manually move the axis away from the Q Setter. Without the Q Setter being wired to the Skip Signal Input, the same will happen when using G31. The G31 function doesn't see a Skip Signal and therefore, doesn't skip to the next block and the program stalls.

Regards,

Bill

 

[sinha]

I suspect that the Q Setter is not wired to the Skip Signal Input

I am not aware of the hardware arrangement associated with G31, so I have a doubt.
If the Q setter is not wired, then axis movement should not stop upon hitting it?

 

[EKrol]

What value is stored in System Variable #5061 when you execute the program with 1mm subtracted from X492.6115, it should be 491.6115? If so, the G31 function is operating correctly and I suspect that the Q Setter is not wired to the Skip Signal Input. In this case, the machine and control is operating in the same way as when manually jogging the axis onto the Q Setter, the axis travel will be halted and must be manually driven away from the Q Setter..

G31 has all the same attributes as G01 (except an alarm will be raised if G31 is issued in G41/G42 mode. Accordingly, if the axis were to be driven onto the Q Setter using G01 mode, the control would protect itself by hauling axis traverse when any of its switches are made and you would have to manually move the axis away from the Q Setter. Without the Q Setter being wired to the Skip Signal Input, the same will happen when using G31. The G31 function doesn't see a Skip Signal and therefore, doesn't skip to the next block and the program stalls.

Regards,

Bill

The measured value is indeed in #5061 and G31 is working. I think you right that the input from the Q setter does not activate the skip function but going in the protection mode. But i guess this can be solved by changing some parameters? Should i can see in the ladder if the skip function is active?

Gr

 

[sinha]

I guess, some parameter setting is not proper. For example, this one may have a bearing:

It is 6201#7

 

[EKrol]

I guess, some parameter setting is not proper. For example, this one may have a bearing:
View attachment 411084
It is 6201#7

At this moment the 6201 are all zeros looking in the machine backup. Not at the machine right now. Should #7 be 1? There are alot of parameters around this subject. Scared to just change some parameters and crash into the probe. Happened to me once with 48000mm/min. Lucky it was only the breakstem that was broken.

 

[sinha]

I cannot take the risk of advising something which I am not sure of.
But, I think there is no harm in changing it to 1. If it does not help, change it back to 0.
Use a low feedrate and a small overtravel distance, just in case the motion does not stop.

There are a few more parameters to check.

 

[rjwalker1973]

What value is stored in System Variable #5061 when you execute the program with 1mm subtracted from X492.6115, it should be 491.6115? If so, the G31 function is operating correctly and I suspect that the Q Setter is not wired to the Skip Signal Input. In this case, the machine and control is operating in the same way as when manually jogging the axis onto the Q Setter, the axis travel will be halted and must be manually driven away from the Q Setter..

G31 has all the same attributes as G01 (except an alarm will be raised if G31 is issued in G41/G42 mode. Accordingly, if the axis were to be driven onto the Q Setter using G01 mode, the control would protect itself by hauling axis traverse when any of its switches are made and you would have to manually move the axis away from the Q Setter. Without the Q Setter being wired to the Skip Signal Input, the same will happen when using G31. The G31 function doesn't see a Skip Signal and therefore, doesn't skip to the next block and the program stalls.

Regards,

Bill

So it is working like the protected move in probe routines to prevent damage?

 

[rjwalker1973]

I cannot take the risk of advising something which I am not sure of.
But, I think there is no harm in changing it to 1. If it does not help, change it back to 0.
Use a low feedrate and a small overtravel distance, just in case the motion does not stop.

There are a few more parameters to check.

I was wondering about the chances of it breaking the tool setter stylus.

 

[EKrol]

I cannot take the risk of advising something which I am not sure of.
But, I think there is no harm in changing it to 1. If it does not help, change it back to 0.
Use a low feedrate and a small overtravel distance, just in case the motion does not stop.

There are a few more parameters to check.

i will try this tomorrow at the machine. Thank you

 

[rjwalker1973]

i will try this tomorrow at the machine. Thank you

Both of these guys know there stuff. Bill everyday and Sinha on Mondays, Wednesdays, Fridays and 35 minutes on Sunday morning. Just kidding Sinha

 

[angelw]

I am not aware of the hardware arrangement associated with G31, so I have a doubt.
If the Q setter is not wired, then axis movement should not stop upon hitting it?

Think about it logically Sinha, most Q setters are used by manually movement of the axis, with the axis being driven towards the Q setter via manual feed at a parameter set feed rate. In this case, G31 doesn't even enter the conversation. With the Q Setter in place for measurement, you can drive the axis towards it from any distance away and via any mode and by manually actuating the switch of the Q Setter, axis movement will be halted.

I have many clients with lathes Not equipped with User Macro but have Q Setters for Tool Setting. They all have the G31 code available, but it requires User Macro to do anything with the possibility of a Skip Signal being raised. All of these machines act in the same manner as the OP's if the switch of the Q Setter is made by driving the axis with G31. The axis movement is halted and the program ceases to proceed.

So it is working like the protected move in probe routines to prevent damage?

It would be a lame PMC program that didn't stop axis movement for an inadvertent actuation of the Q Setter switch. These systems are normally wired so that the circuit has to be interrupted, so that they fail safe. If the wires to the system are broken, its the same as actuating the Q Setter Switch with regards to stopping axis movement.

Regards,

Bill

 

[rjwalker1973]

It would be a lame PMC program that didn't stop axis movement for an inadvertent actuation of the Q Setter switch. These systems are normally wired so that the circuit has to be interrupted, so that they fail safe. If the wires to the system are broken, its the same as actuating the Q Setter Switch with regards to stopping axis movement.

Regards,

Bill

Gotcha. Thanks Bill

 

[sinha]

Both of these guys know there stuff. Bill everyday and Sinha on Mondays, Wednesdays, Fridays and 35 minutes on Sunday morning. Just kidding Sinha

I do know quite a few things, but Bill is at a different level !