[oldgoat]

After lurking in the forums for a while, I would just like to say I am amazed at the amount of knowledge and the helpful attitude of the members of CNC Zone.

That being said, I was hoping to find some more knowledge about the inner workings of Tool Length Measurement B as it pertains to a Fanuc 15MA. I have read numerous times the information I can find in the Series 15-MA, 15-MF, 150-MA Operator's Manual (B-61224E/07) on how the function is supposed to work from the operator's point of view and it is pretty much cut and dry. I also have read the information I could find in the Series 15/150 Model B BMI Interface Connection Manual (GFZ-62073E-1/04), which may or may not apply. I also used any information I could extract from the PMC Ladder Language Programming Manual (Vol 1) (GFZ-61863E/14) which does NOT include any information for the PMC-N, so it may or may not apply. I do NOT have the Series 15 Model A BMI Interface Connection Manual to look through. I have found a detailed description of the interface requirements for Tool Length Measurement B as it works for a lathe in a Series 15B in the 15B BMI Connection Manaul, but I am not sure how this pertains to or translates over for operation on a Series 15A mill. I have included the relevant pages from the 15B BMI manual as an attachment below.

I have also included the relevant pages from the 15MA Operator's Manual as an attachment below. I guess my questions are:

1) When the "TOOL LENGTH MEASUREMENT" switch on the machine side as described in the operator's manual (Page 568) is turned on, what happens next? At this point, is the GOQSM (G028.7) signal asserted by the PMC as in the description for the lathe system in the 15B BMI manual?

2) Do the +MIT1~3 and -MIT1~3 apply to the 15M as well as the 15T as described in the 15B BMI manual?

3) Since I did not find a detailed description of how the TLMB function works for a 15M series, does one exist?

I apologize for the long winded post. I just wanted to make sure I had all my thoughts together correctly and explained it in the same way.

Thanks for any help in advance...

Ken

[Al_The_Man]

According to my 15MA Operator manual, there is a detailed description of TLMB in section 10.9. ?
The last Fanuc system I installed was a 15A before switching over to exclusively Mitsubishi so I am a bit rust on it.
Al.

[oldgoat]

Al,

While there is a detailed description of how TLMB works in the Operator's Manual from an operator's point of view, it does not describe any of the details of what happens "behind the panel" when one invokes this function (The pages you described are one set of the pages I attached to the original post). I was hoping for more of a step by step "behind the panel" sequence of events as it pertained to using it on a mill, or 15M system. This type of description which I found was for a lathe, or 15T series, included as the other attachment in the original post, and I do not know how it pertains to or translates to using it on a 15M series. The description specifically calls out and shows an example with CNC and PMC signals as it relates to the 15T and 15TT.

Ken

[Al_The_Man]

I will check the docs I have a bit further.
I noticed that there is a 9000 option par for Tool Length Measurement?
Al.

[oldgoat]

I noticed that there is a 9000 option par for Tool Length Measurement?

As well as a few other things which need to be worked around. I do not want to get into a discussion of why it cannot be done, or why it could not be done, as well as posting proprietary information. I just would like to learn how it integrates into the machine tool, and how it works from the machine tool and CNC point of view. This definitely and undeniably has to be the easiest, quickest, least error prone way of setting tool lengths on a HMC.

Thanks,
Ken

[angelw]

I noticed that there is a 9000 option par for Tool Length Measurement?

As well as a few other things which need to be worked around. I do not want to get into a discussion of why it cannot be done, or why it could not be done, as well as posting proprietary information. I just would like to learn how it integrates into the machine tool, and how it works from the machine tool and CNC point of view. This definitely and undeniably has to be the easiest, quickest, least error prone way of setting tool lengths on a HMC.

Thanks,
Ken

Tool length measurement on Fanuc controls use the skip function G31 to feed the tool onto a mechanical switch. Axial motion is like G01 following the G31 command. If an external skip signal is input during the execution of this command, the execution of the command is interrupted and the next block is executed. A target coordinate is used that is beyond the physical location of the switch that will apply the skip signal, and basically the tool being measured runs into the switch on its way to the commanded coordinate.

The implementation of a tool length measuring system would vary according to the hardware manufacturer, but the overall scheme is similar. The Renisahw system uses a normally closed switch and looks for this condition before allowing the tool to approach. This guards against problems such as broken wires etc. The tool advances at a relatively high feed rate until contact with the switch is made and hence, initiates the skip signal. The tool is normally then moved a short distance away from the switch and another contact is made under G31 command at a slower feed rate to gain a more accurate position at which the interrupt occurred.

A User Macro program is used to interpret the state of the switch and to apply some simple mathematics to calculate the tool length based on the Machine Coordinate when the interrupt signal occurred, and to load the resulting tool length into the appropriate offset registry.

Tool length/diameter measuring equipment is not overly difficult to install as an after market device.

Regards,


Bill

[Al_The_Man]

Looking through the Fanuc manuals, which are slightly better than the older systems but still not very clear what is required.
It seems to me that the TLMB can be entered two ways?
One manually through softkeys and automatically by tool setter by setting BMI-DI internal register G08.5 (PRC), this would be set via a PMC input, which does not appear to have a dedicated input assigned to it.
The rung would need to be added to the PMC.
I am also assuming by exercising a G code G37 the tool move to the presetter position and waits for the PRC signal, similar to G31?
I have never done it on a 15, so it is just an assumption from what can be gleaned from the manuals?.
There is also a series of user parameters for setting the TLMB, in 6000's I believe.
Al.

[oldgoat]

Looking through the Fanuc manuals, which are slightly better than the older systems but still not very clear what is required.

My guess is clear was a relative term for the manual writers at Fanuc.

There is also a series of user parameters for setting the TLMB, in 6000's I believe.

From what I could gather, the following parameters need to be set in conjunction with TLMB for a Series 15M:

6002.6 [QNI]

QNI Specifies the method used to set the tool offset number when measured tool offset input function B
(only for the Series 15–T and 15–TT) or tool length measurement function B (only for the Series 15–M)
is used.

0 : Select tool offset No. with cursor on MDI/CRT unit.

1 : Tool offset number is set by a signal from the machine.

I would be selecting option 0, select the offset on the offset screen.


6003.0 [TC2] & 6003.1 [TC3]

TC3 TC2 Meaning
0 0 Tool change position is the 1st reference point
0 1 Tool change position is the 2nd reference point
1 0 Tool change position is the 3rd reference point

Our particular machine uses G30 for the tool change position, so I would have to select 01.


6003.2 [TMA]

TMA Specifies the axis for which tool length is measured.

0 : Measure tool length along the Z–axis.

1 : Tool length can be measured for any axis.

Not sure which way to go yet, but most likely option 1.

6024

This parameter is used by function B for measuring tool length/workpiece origin.
For each axis, set the distance from the reference tool tip to the reference measurement surface (L in the figure
below) when the machine is at the machine origin.

Those are the parameters I found listed in the Fanuc Series 15/Fanuc Series 150 Operator's Manual (Appendixes) (B-61220E/05)

Now for the first step, I need to know what the switch in the following text (which was extracted from the Series 15 Operation Manual for Machining Center) does as far as signal input. Obviously the switch is an input to the PMC, probably a non-dedicated input. When the PMC receives this input, and the mode is in handle or jog (manual continuous feed), what signal does the PMC send to the CNC??

(Extracted directly from the FANUC Machining Center Operator's Manual)
Procedures for measuring the tool length compensation value

1 Move the machine to the tool change position by manually returning to the reference position.
2 Select the manual handle feed or continuous manual feed mode.
3 Turn on the “TOOL LENGTH MEASUREMENT” switch on the operator’s panel on the machine. The control
unit then automatically changes the CRT screen to that for measuring the tool length compensation
value, shown on the next page. The OFST status display blinks at the bottom of the screen to indicate that
the preparation for measuring the tool length compensation is completed.

That is step one. My guess is there will be more. Once again, I apologize for the long winded post. I hope my thoughts came through clearly.

Ken

[angelw]

My guess is clear was a relative term for the manual writers at Fanuc.



From what I could gather, the following parameters need to be set in conjunction with TLMB for a Series 15M:

6002.6 [QNI]

QNI Specifies the method used to set the tool offset number when measured tool offset input function B
(only for the Series 15–T and 15–TT) or tool length measurement function B (only for the Series 15–M)
is used.

0 : Select tool offset No. with cursor on MDI/CRT unit.

1 : Tool offset number is set by a signal from the machine.

I would be selecting option 0, select the offset on the offset screen.


6003.0 [TC2] & 6003.1 [TC3]

TC3 TC2 Meaning
0 0 Tool change position is the 1st reference point
0 1 Tool change position is the 2nd reference point
1 0 Tool change position is the 3rd reference point

Our particular machine uses G30 for the tool change position, so I would have to select 01.


6003.2 [TMA]

TMA Specifies the axis for which tool length is measured.

0 : Measure tool length along the Z–axis.

1 : Tool length can be measured for any axis.

Not sure which way to go yet, but most likely option 1.

6024

This parameter is used by function B for measuring tool length/workpiece origin.
For each axis, set the distance from the reference tool tip to the reference measurement surface (L in the figure
below) when the machine is at the machine origin.

Those are the parameters I found listed in the Fanuc Series 15/Fanuc Series 150 Operator's Manual (Appendixes) (B-61220E/05)

Now for the first step, I need to know what the switch in the following text (which was extracted from the Series 15 Operation Manual for Machining Center) does as far as signal input. Obviously the switch is an input to the PMC, probably a non-dedicated input. When the PMC receives this input, and the mode is in handle or jog (manual continuous feed), what signal does the PMC send to the CNC??



That is step one. My guess is there will be more. Once again, I apologize for the long winded post. I hope my thoughts came through clearly.

Ken

Ken,
What you're referring to, I believe, is the Tool Length Measuring feature where the tool is moved manually to a reference of known height, and a once there a Measure hard or soft key pressed to initiate the measurement of the tool. If this is the case, and your machine does not have this feature, but has the User Macro, then you can achieve the same thing, only better in my opinion, by obtaining or writing a User Macro program for tool length measurement. The same applies for Work Shift setting. All of this can be achieved without PMC ladder modifications and generally without parameter changes.

What I described in my original reply was Automatic Tool Length measurement, were the tool is presented to a measuring probe under program control. This feature has many advantages, such as periodic measurement of the tool in cycle to determine tool wear, and presenting tools that have performed critical operations to determine if they broke during their cycle. An example of this would be a drilled and tapped hole. The drill can be presented to the setting probe, and if broken, trying to tap the non existing hole can be avoided.

Regards,

Bill

[oldgoat]

What you're referring to, I believe, is the Tool Length Measuring feature where the tool is moved manually to a reference of known height, and a once there a Measure hard or soft key pressed to initiate the measurement of the tool. If this is the case, and your machine does not have this feature, but has the User Macro, then you can achieve the same thing, only better in my opinion, by obtaining or writing a User Macro program for tool length measurement. The same applies for Work Shift setting. All of this can be achieved without PMC ladder modifications and generally without parameter changes.

Bill,
You are exactly correct. We currently have two HMCs, and setting tool length offsets can be a real bear for the uninitiated, as well as for us initiated types. We regularly machine multiple parts in multiple operations on multiple sides of the tombstones, and use a macro for setting our work offsets since we far exceed the 6 available. This also aids in change overs, since all the work coordinates are preset in the programs, and rarely change much (if at all) from run to run. One has to be real careful when picking the point for touch off for tool replacement. While both machines already have the "regular" tool length measurement option, you have to make sure you pick the correct offset on the correct face of the tombstone and touch off the correct face of the part. All told, too much room for error. Tool Length Measurement B allows a fixed and permanent reference point to be set in parameters, have the operator flip a switch and be presented with the tool offset screen, jog and handle to the "touch off" point, cursor to or otherwise select the correct tool height offset, press measure, done. While I am not against doing this with a macro, it just seems to be intuitively simpler with TLMB.

What I described in my original reply was Automatic Tool Length measurement, were the tool is presented to a measuring probe under program control. This feature has many advantages, such as periodic measurement of the tool in cycle to determine tool wear, and presenting tools that have performed critical operations to determine if they broke during their cycle. An example of this would be a drilled and tapped hole. The drill can be presented to the setting probe, and if broken, trying to tap the non existing hole can be avoided.

This would be the next logical progression after TLMB. I need to check more into the hardware, as both HMCs are not exactly the same. One already has installed, is set up for a probe, but we have no probe. It uses a Wako UTS. The other has a Probe, but looks like the internal interface hardware is missing. One thing at a time...

I appreciate your input, and am more than willing to accept any more knowledge you may wish to share.

Ken

[angelw]

Bill,
Tool Length Measurement B allows a fixed and permanent reference point to be set in parameters, have the operator flip a switch and be presented with the tool offset screen, jog and handle to the "touch off" point, cursor to or otherwise select the correct tool height offset, press measure, done. While I am not against doing this with a macro, it just seems to be intuitively simpler with TLMB.

Ken,
I've set many machines up to do semi automatic tool length measuring, as have many of the contributors to this forum, based on some of the threads I've followed, and I still feel that a well implemented User Macro system is better than TLMB.

One system I've implemented in the past is launched via MDI using a User Defined G Code. This G Code calls the Macro program and passes a parameter in the way of a tool number, to set just one tool, or a start and end tool number, to set a range of tools. The action of this Macro program is to position the tool at the tool set position in X and Y and then display a message instructing the operator to manually touch off the tool on the setting device, be it a dial indicator type device, or a block of material of known height. Once correctly positioned in Z,the cycle start button is pressed in MDI mode and the calculated tool length is registered in the correct offset record based on the current spindle tool number. The process is completed by the tool returning automatically to the Z Reference point.

Regards,

Bill

[derekBPcnc]

Ken,

One system I've implemented in the past is launched via MDI using a User Defined G Code. This G Code calls the Macro program and passes a parameter in the way of a tool number, to set just one tool, or a start and end tool number, to set a range of tools................
Regards,
Bill

Hi Bill,

Would you be willing to share the macros? :cheers:
At the moment, I'm setting TLOs with a dial gauge, but by thrashing the HMI buttons manually
ATB
Derek

[angelw]

Hi Bill,

Would you be willing to share the macros? :cheers:
At the moment, I'm setting TLOs with a dial gauge, but by thrashing the HMI buttons manually
ATB
Derek

Hi Derek,
No problems. However, I'm just about to walk out the door to catch a plane, and I need to find the code on another computer. I'll be back on Sunday and will post it then.

Regards,

Bill

[stevo1]

Bill,
While I am not against doing this with a macro, it just seems to be intuitively simpler with TLMB.
Ken

Ken,
I have to agree with Bill on this for sure. I have written quite a few TLM macros on tool setters. The best way is as Bill described. I setup a custom G or M code to automatically call the macro program. The tool setter is in a fixed location and does not move. You must have a setting that tracks the current tool in the spindle. Say you set it up with a custom G-code of G37. You can just program in MDI G37 and it will automatically touch off the tool and place the tool geometry in the offset page. No manual moving of tools, no shimming of tools on the table, no pushing the measure function and the best part is no one can accidentally make a mistake of touching off on a part and using the + or - in the wrong direction.

It is as error proof and hands free as it gets.

You can even go as far as putting the G37 in a tool change program so every time a tool is called it touches it off.

Stevo

[derekBPcnc]

Hi Derek,
No problems. However, I'm just about to walk out the door to catch a plane, and I need to find the code on another computer. I'll be back on Sunday and will post it then.
Regards,
Bill

Thanks,
Safe travels,
Derek