[ecapatto]

Dear colleagues,

We have one machine here that was conventional and now we put one old (very old) FANUC 16-TB on that.

The machine is fully parametrizated as well as drives and control itself, tool changes, the machine works fine, back lash and lead screw table are setted and everything is fine. BUT

The values on Geometry and in the Wear aren't updating the absolute coordinate system. To be able to evaluate the machine geometry and make some machining tests I had to insert the Tool Geometry Values on Work Offset, and then work with just one tool.

Even the Wear isn't working. The screen is there, the measure - insert c - insert + and input are avaliable, the values are inserted correctly using the insert c, but when I program T0202 the change occurs but the values of absolute isn't working.

Need help because I think that this function is on basic software package.

If you can help me again I'll be glad.

[stevo1]

Take a look at the attached PDF parameter 3104 settings it shows the parameter setting for the display to use or not use the tool offset. This is probably your problem.

Stevo

[ecapatto]

Hi Stevo,

I'll try this parameter right now! I saw that this parameter is related with par 5002 so I'll check the both.

Thank you by the advance.

[stevo1]

Your welcome.

Stevo

[ecapatto]

I'd tried the parameter and nothing changes. Still not updating Abs values when T0202 or any other tool is called.

Can the tool change routine O9000 making something wrong? I mean, there is no more parameters to control Wear / Geom behavior.

A friend that was FANUC employee (the guy that wrote the ladder for this machine) told me some days ago that it can be a FANUC basic software issue that can be solved only changed the CNC EPROM where it's recorded.

I have doubts about that, because it's soo simplest, It's just about program the T code and the values must be updated. I've never saw one CNC with this behavior before. My guess is that the tool change routine is making some mistake and not leaving the control to update the values.

[stevo1]

Can you post the 9000 tool change macro?

You have the parameters set to use the last 2 digits as the offset value correct?

Is the machine actually instating the tool offset and just not showing it on the program check screen?

Stevo

[sinha_nsit]

Dear colleagues,

To be able to evaluate the machine geometry and make some machining tests I had to insert the Tool Geometry Values on Work Offset, and then work with just one tool.

Not very clear what you are doing.
If you are setting G54 work offset with one tool by touching off and measuring, you do not need any geometry offset for this tool. Can call this tool just by T0200 or T200 (assuming it is tool number 2).
If you want to use T0202, the corresponding geometry offset (in row number 2) should be zero.

[ecapatto]

Stevo:
- I'll try to post the tool change macro
- The parameters set the Offset correctly, to use last two digits
- No, the machine isn't updating the values, I have one test NC program to evaluate this situation.

The T0202 appears on lower right corner in the screen, like it's active, but it isn't.

Sinha_nsit:
- I did changes on work zero (G54) to evaluate the machine geometry, because it was refoubished. But in the normal operation the operator needs to insert the correspondent data for each tool in each Geometry screem row.
- Working like I did just allow operator to use G54 for tool 1, G55 for tool 2 .... It isn't the correct way. The correct way is to have G54 set up to workpiece end face, or chuck face or wherever they want and the tool geometry relative to that position. But FANUC isn't taking into account the value on that screem [WEAR/GEOM], I dont't know why.

Even the Wear aren't working, as I told, I never saw one FANUC controller acting like this one.

[ecapatto]

Follow the Macro fot Tool Change: PLEASE HELP-ME

FYI, the machine FANUC control have two channels, the second isn't in use.

%
O9000(TOOL CHANGE)
N10#110=#4001
N20#111=#4002
N30#112=#4003
N40#500=FIX[#149/100.0]
N50IF[#500GT8.0]GOTO1230
N60IF[#500EQ#501]GOTO1300
N70IF[#501EQ0]GOTO500
N80G91G0G28Z0
N81G90G0B[#501*45.0]
N85G4P400
N90IF[#1000EQ1]GOTO1240
N100G91G30X0
N110M50M53M54
N120G4P500
N130M52
N140G4P500
N150M55
N160#501=0.0
N170G90
N180IF[#1000EQ0]GOTO1260
N500IF[#500EQ0]GOTO1110
N510G91G28Z0
N515G90G0B[#500*45.0]
N520G91G30X0
N530G4P500
N540IF[#1000EQ0]GOTO1250
N550M50
N560M54
N570G4P500
M580M51M53
N590#501=#500
N600G4P500
N610M55
N1100G#110G#111G#112
N1110M51
N1120M99
N1230#3000=1(WRONG T VALUE)
N1240#3000=2(OCCUPED POSITION)
N1250#3000=3(NO TOOL AN THIS POSITION)
N1260#3000=4(TOOL NOT OUT)
N1300M99
%

[sinha_nsit]

Simple first:
Call tool number 1 by
G54;
T100;
Does it work correctly?

If yes, make geometry and wear values in row number 1 equal to zero. (You would need to edit both geometry and wear screens one-by-one, which can be selected by softkeys).
Now call tool 1 by
G54;
T101;
Does it work correctly (should be exactly same as previous case)?

[sinha_nsit]

Use of #149 indicates that you are calling a sub by a T-code. Such a T-code in the main program does not have tool-change function; it just calls a sub 9000 (no other sub can be called). So, you need to insert T#149 in the sub, wherever you want a tool change (say, after homing). The T-code in the sub behaves like the usual tool-change code. Your sub does not have T#149 anywhere.
(If you command T101 in the main program, 101 automatically gets stored in #149 for use in sub)

Ignore my previous post.

[stevo1]

Sinha....regardless of #149 when you program a T0101 offset 01 should be taken into account correct??

I am a bit stumped on this one right now. Let me do some thinking on this one.

Stevo

[dcoupar]

Use of #149 indicates that you are calling a sub by a T-code.

I believe this is only true if parameter 6001 bit 5 is set to 1. If 6001.5=0, a T-code in the main program is just a T-code.

[ecapatto]

Dear colleagues,

I'd changed the Tool Cnage Macro inserting the code T#149 before M99 and the machine just stop at that block, start still green and nothing happens.

The actual related parameters are (in machine):

#6001.0 = 0
#6001.1 = 0
#6001.2 = 0
#6001.3 = 0
#6001.4 = 0
#6001.5 = 1
#6001.6 = 1
#6001.7 = 0

#5002.0 = 1
#5002.1 = 0
#5002.2 = 0
#5002.3 = 0
#5002.4 = 0
#5002.5 = 0
#5002.6 = 0
#5002.7 = 0

#3104.0 = 1
#3104.1 = 0
#3104.2 = 0
#3104.3 = 0
#3104.4 = 1
#3104.5 = 0
#3104.6 = 1
#3104.7 = 0

I have a guess of what is going on. I want to unrrelate the Tool Cnage macro from T code and assign this to M6 code.

Assign the O9000 to M6 is quite easy, but how can I separate the O9000 from T code?

Or if one of you have a better idea, I'm listening.

Regards,

[sinha_nsit]

I believe this is only true if parameter 6001 bit 5 is set to 1. If 6001.5=0, a T-code in the main program is just a T-code.
Right

regardless of #149 when you program a T0101 offset 01 should be taken into account correct??
If 6001#5 is set to 1, the T-code loses its tool-change function in the main program. It just calls O9000. In O9000, it acquires tool-change function. The best thing would be to test it:
Set 6001#5=1 (edited)
Have only M99 in O9000
Now command T0101 or T0202 or any other number you wish.
Nothing would happen.
This is described in quite detail on pp. 150-151 of my book on macro. I have attached these pages for those who do not have this book.

I'd changed the Tool Cnage Macro inserting the code T#149 before M99 and the machine just stop at that block, start still green and nothing happens.
Set 6001#5=0 and command T0101 (no M30) in MDI. Does it take effect?
If yes, set 6001#5=1 and again execute T0101. Does it work?
If not, post your main program as well as modified O9000.

how can I separate the O9000 from T code
Set 6001#5=0

[stevo1]

Dave…yes with the 6001.5 set proper parameter set it will call a sub with a T() call and set #149 to the modal T(). My assumption would be that no matter what this parameter is set to it should not affect the instating of the tool offsets.

I never use the T() subcall for tool change. I always use a custom M6 to do so.

Ok so are you still having problems with your original question of the tool offsets not instating?? Calling a macro with T() or M6 is not going to change the fact that your offsets should instate no matter what.

Stevo

[dcoupar]

Dave…yes with the 6001.5 set proper parameter set it will call a sub with a T() call and set #149 to the modal T(). My assumption would be that no matter what this parameter is set to it should not affect the instating of the tool offsets.

I never use the T() subcall for tool change. I always use a custom M6 to do so.

Ok so are you still having problems with your original question of the tool offsets not instating?? Calling a macro with T() or M6 is not going to change the fact that your offsets should instate no matter what.

Stevo

It's as sinha_nsit stated in an earlier post.

T101 in the main stores 101 in #149 and calls O9000. It does NOT perform a toolchange or turret index, and does NOT activate any offsets.

To activate the offsets, there has to be a T#149 in O9000 somewhere.

[ecapatto]

We got some progress here.

In both cases, using M6 to call the Tool Change sub (pars 6001.5=0 and #6071=6) or inserting the T#149 into O9000 the Absolute Value now is taking in account the Geometry and Wear values.

The problem now is:
When par 6001.5=0 then there is no association with T and O9000 in MDI mode the control update the absolute values (taking in account the Geom/Wear) and stops at this single block. The cycle start led still on, no alarm raises. The control just stops, but now at least we know that there isn't nothing wrong with the control, just with the guy behind him(nuts).

Any suggestion why the control stops at T command? Even withoout connections with the Macro?

Thanks by the advance,

[dcoupar]

We got some progress here.

In both cases, using M6 to call the Tool Change sub (pars 6001.5=0 and #6071=6) or inserting the T#149 into O9000 the Absolute Value now is taking in account the Geometry and Wear values.

The problem now is:
When par 6001.5=0 then there is no association with T and O9000 in MDI mode the control update the absolute values (taking in account the Geom/Wear) and stops at this single block. The cycle start led still on, no alarm raises. The control just stops, but now at least we know that there isn't nothing wrong with the control, just with the guy behind him(nuts).

Any suggestion why the control stops at T command? Even withoout connections with the Macro?

Thanks by the advance,

If you simply MDI T101 and cycle start that, does it pick up the offset? What kind of machine is this?

[sinha_nsit]

If using M6, which would call O9001 (with your parameter setting) as a subprogram, you need to insert the complete T-code, such as T0101, in O9001. Not a good idea.

Therefore, you need to use M6 for calling a macro where you would be able to pass data to the macro. For this,
Reset 6071, and set 6080=6.Then M6 would call O9020 as a macro.
In the main program, command M6 T0101 (not T0101 M6), and insert T#20 somewhere in O9020.
For more information, read the attachment.

Sinha