Fanuc 10t/15t lv-24m-ma

[jovica]

I need to setup this machine. I've created a program and on simulation it's working.

X, Y, Z, C axis are set to zero. I can move all axis and i can turn on spindle.

M55 for turning (C axis)
S10000 M04
this is ok but

when i want to call a tool like T2401 it says Program not found!

Is it possible that i've erased some macro program from memory, and can i write it back?

And one silly question: Is there a reset button to factory default?

Thanks!

[angelw]

Originally Posted by jovica

I need to setup this machine. I've created a program and on simulation it's working.

X, Y, Z, C axis are set to zero. I can move all axis and i can turn on spindle.

M55 for turning (C axis)
S10000 M04
this is ok but

when i want to call a tool like T2401 it says Program not found!

Is it possible that i've erased some macro program from memory, and can i write it back?

And one silly question: Is there a reset button to factory default?

Thanks!

1. Take a look at parameter #7000 bit 0. Bit 0 is at the right most end of the byte display and will be labeled TCS. If this bit is set to 1, Sub program O9000 is called in the block in which T is specified.
2. Look for program number O9000 to see if the program exists. You may have to change parameter #2201, bit 0 to 0 to be able to view this program.

Does this machine have a conventional Tool Turret, or is its a magazine type? Because your above example refers to Tool Num 24 and because its uncommon to use a Macro program on a conventional Tool Turret turning centre, I'm guessing the later. If #7000.0 is set to 1, and O9000 does not exist, meaning that somehow its been deleted, it will be difficult to write another program from scratch without knowing exactly what the PLC does in the Tool Change operation and what Interface signals may be used. If #7000.0 is set, indicating that there should be a O9000, and O9000 is gone, I suggest that you contact the MTB, or with a lot of luck, some Forum member with the same type of machine may chime in and send you a copy.

Writing the program from scratch is doable, but you need to be able to read and understand the PLC (PMC) program and electrical schematic drawing.

Regards,

Bill

[jovica]

Thanks for your reply.

It is a Tool Turret (vertical). Turret has turn tools (T21,T22,...) and milling tools(T13, T12,...).

I was testing it. Some tool change, simple turn process and everything was ok and working, but then i wanted to save that programs into memory dir. I cleared everything and saved it (?). Problem is that i can't run that program from memory (sometimes it says "End of record"). After that when i'm in MDI and i want Txxxx there is a error "Program not found". Spindle is working properly.
I have a manual book and some macro programs in it. I will write another post with that macros so you can check. Maybe it is a simple solution but ...

Best Regards,
Jovica

[angelw]

Originally Posted by jovica

Thanks for your reply.

It is a Tool Turret (vertical). Turret has turn tools (T21,T22,...) and milling tools(T13, T12,...).

I was testing it. Some tool change, simple turn process and everything was ok and working, but then i wanted to save that programs into memory dir. I cleared everything and saved it (?). Problem is that i can't run that program from memory (sometimes it says "End of record"). After that when i'm in MDI and i want Txxxx there is a error "Program not found". Spindle is working properly.
I have a manual book and some macro programs in it. I will write another post with that macros so you can check. Maybe it is a simple solution but ...

Best Regards,
Jovica

Hi Jovica,
Post a picture of the Tool Turret, if you don't mind.
How did you go about "Clearing Everything"?

A post of the Macro program will be good. I, or some other Forum member will be able to help I'm sure.

Check out what I advised regarding parameter #7000.0 and program O9000 and let us know what you find.

Regards,

Bill

[jovica]

By the end of the week i will try your advice regarding parameter and program.

About "Clearing Everything" i wanted to delete saved program in memory (only one as i recall) so i pressed delete -> All. Now dir memory is empty and when i save some program it is listed in memory.
Is it possible that i have erased tool change program from memory?

Insted of a picture i found this:
http://www.youtube.ug/watch?hl=en-GB&v=lxU4TKz_5Tc
On one side milling tools(i think they are T11-T16) and on other turning tools( T21-T26)

And here is macro.
-Custom macro programs:
Main program
O9000
G0G40
#1132=0
#130=BCD[#149]
#134=#130AND65280
#135=#130AND255
#132=BIN[#134]
#133=BIN[#135]
IF#132EQ3100GOTO200
IF#132EQ3400GOTO300
IF#132EQ3000GOTO400
#136=#149
T#136
GOTO500
N200IF=133EQ#500GOTO500
IF#133EQ#501GOTO600
IF#1003EQ1GOTO200
M98P9023
GOTO500
N300IF#133EQ#501GOTO500
IF#133EQ#500GOTO600
IF#1003EQ1GOTO300
M98P9024
GOTO500
N400
IF#1003EQ1GOTO400
M98P9020
N500M99
N600#3000=199(MAGAZINE ERROR)
M30


With this main program i have:
Magazine control program O9020,
Milling tool change program O9023,
Turning tool change program O9024,
Arm return program O9009

Best regards,
Jovica

[angelw]

Originally Posted by jovica

By the end of the week i will try your advice regarding parameter and program.

About "Clearing Everything" i wanted to delete saved program in memory (only one as i recall) so i pressed delete -> All. Now dir memory is empty and when i save some program it is listed in memory.
Is it possible that i have erased tool change program from memory?

Insted of a picture i found this:
http://www.youtube.ug/watch?hl=en-GB&v=lxU4TKz_5Tc
On one side milling tools(i think they are T11-T16) and on other turning tools( T21-T26)

And here is macro.
-Custom macro programs:
Main program
O9000
G0G40
#1132=0
#130=BCD[#149]
#134=#130AND65280
#135=#130AND255
#132=BIN[#134]
#133=BIN[#135]
IF#132EQ3100GOTO200
IF#132EQ3400GOTO300
IF#132EQ3000GOTO400
#136=#149
T#136
GOTO500
N200IF=133EQ#500GOTO500
IF#133EQ#501GOTO600
IF#1003EQ1GOTO200
M98P9023
GOTO500
N300IF#133EQ#501GOTO500
IF#133EQ#500GOTO600
IF#1003EQ1GOTO300
M98P9024
GOTO500
N400
IF#1003EQ1GOTO400
M98P9020
N500M99
N600#3000=199(MAGAZINE ERROR)
M30


With this main program i have:
Magazine control program O9020,
Milling tool change program O9023,
Turning tool change program O9024,
Arm return program O9009

Best regards,
Jovica

Hi Jovica,
The video was very helpful, and I can understand why a Macro program may be required for this type of tool changer. Why I say "may" is that all could have been accomplished in the PLC, but most MTBs tend to allow the NC side of the control do some of the work.

Check out parameter #2201, bit 0. If this is set to 0, then yes, there is a possibility that you deleted the O9000 - O9999 programs. This bit Enables/Disables editing (which includes deleting) of programs in the aforementioned range.

Its fortunate that you have hard copies of the Macro programs as this Macro would have been difficult to write from scratch without a good understanding of the PLC program. A generic Tool Change program would not have helped.

The fact that the "Program not found" alarm is being raised, would indicate that #7000.0 is set. The program block in O9000, #130=BCD[#149], further reinforces the fact that #7000.0 should be set to 1. As explained in my earlier Post, setting this bit enables O9000 to be called with a T code. When calling O9000 with a "T" code, the tool number is stored in Common Variable #149. I believe that loading the Macro programs (all of those listed) again will resolve your issue. Make sure you set #2201.0 to 1 after you load and confirm that all is OK. This will prevent deletion of the programs again.

Let us know how you get on.

Regards,

Bill

[jovica]

Hi Bill,
I loaded all macro programs and it worked
I tried to lock them with #2201 parameter but it says "write protected" (can't change from bit 0 to 1). Maybe there is a switch or some other parameter to check. That's not very important at this time.

I have one more question. It's tool measuring (tool offset)? I can manually measure it from work piece to tool(zero return-machine) and then write it to offset and it is working. There is "direct input of offset measured" but i didn't figured it out.

Thank you very much!
Best regards,
Jovica

[angelw]

Originally Posted by jovica

Hi Bill,
I loaded all macro programs and it worked
I tried to lock them with #2201 parameter but it says "write protected" (can't change from bit 0 to 1). Maybe there is a switch or some other parameter to check. That's not very important at this time.

I have one more question. It's tool measuring (tool offset)? I can manually measure it from work piece to tool(zero return-machine) and then write it to offset and it is working. There is "direct input of offset measured" but i didn't figured it out.

Thank you very much!
Best regards,
Jovica

Hi Jovica,
In Fanuc manuals I have for your model control, it shows parameter #2201.0 as the bit to enable/disable the editing of programs in the number range O9000 to O9999. The correct bit to change to protect these programs is labeled NE9. If your control parameters are different to what I'm specifying, find the parameter that has a bit labeled NE9 to protect the O9000 to O9999 programs, but I'm confident that #2201.0 is correct. What you're confusing it with is a System Variable for Tool compensation. Accordingly, look in the parameter section of your manual, and also look at parameter #2201 in your control to see what I mean.

To be able to change a parameter, you have to set Parameter Write Enable (PWE). With a Series 10 - 15 control the procedure is as follows:

1. Select MDI Mode
2. Press the Software Key SETTINGS to select the settings screen
3. Enter 8000
4. Press the Software Key INP-NO. Parameter 8000 is displayed
5. Enter 1 and press the INPUT Software Key. PWE=1 is specified and parameters can now be modified. The control enters an alarm status, alarm 100. Ignore this and go to the required parameter page to make changes.
6. When finished making parameter changes, PWE needs to be set back to 0. Follow the instructions 1 to 5, but enter 0 in step 5.
7. After PWE is set to 0, press reset to clear the alarm.
8. Some parameters require that the control be cycled through shut down and restart.


Regards,

Bill

[jovica]

Ok. I will try it.

Regards,
Jovica

[jovica]

Hi Bill,
Locking was successful!
Now i have another problem After creating a program, it is impossible for me to set work piece zero (G54, G55...) and tool offset. I tried to measure it manually. From work piece to my selected tool, then i write it in tool offsets, but G54 is 0,0,0 so it's not working. I can't figure it out. Is there another way to accomplish this. Can you explain to me?

My program is in attachment. Simple turning process.

Best Regards,
Jovica

[angelw]

Originally Posted by jovica

Hi Bill,
Locking was successful!
Now i have another problem After creating a program, it is impossible for me to set work piece zero (G54, G55...) and tool offset. I tried to measure it manually. From work piece to my selected tool, then i write it in tool offsets, but G54 is 0,0,0 so it's not working. I can't figure it out. Is there another way to accomplish this. Can you explain to me?

My program is in attachment. Simple turning process.

Best Regards,
Jovica

Hi Jovica,

Yes I can explain it to you, but first I need you to tell me what features your control has.
1. With regards to setting Geometry Offsets for your turning tools, is there a Measure function associated with the Offset Page.
2. Is there a measure function associated with the G54 to G59 Offset Page
3. What tool numbers and offsets are used for the turning tools
4. What tool numbers and offsets are used for the milling tools
5. How are you setting the Geometry Offsets for your turning tool now.

We know that your machine has the Fanuc User Macro option. Accordingly, if there is no measure function on your machine, I'll show you how to create a User Macro program to set Tool Offsets and and Work Shift Offsets that will be semi-automatic. This method will speed up your Tool and Work Shift setting, as well as eliminate a great deal of potential human error.

Regards,

Bill

[jovica]

Hi Bill,

I have a measure function (button) but i'm not sure what for(i believe it's for tool geometry offset). When i press it, it says "Key no data"(something like that )

For turning tools: T11, T12, T13, T14, T15, T16
For milling tools: T21, T22, T23, T24, T25, T26
Offset for them: Because tool is called with T1101, these two last numbers are offset, i think offset is unique for all of them. I just need to be careful not to mix them. I can't use tool offset 33 for T12 and T13, if you know what i mean.

My way:
I choose a tool let's say T1233. G54 is set to 0,0,0,0. My tool geometry offset (No. 33) is X0,Y0,Z0,R0,Q0. Now when i start my program( i think it goes from machine zero G28 U0. G28V0. G28) i see how much i need to add (+-) in that tool offset to get to the top of my work piece. And somehow it works.

It is too slow. If i have G54 in program it's useless. I thought i can set G54 offset and tool offset like in HaaS VF4 with 3D taster. I know that this Fanuc is an old machine but i believe there is faster way to do this, somehow.

Regardss,
Jovica

[angelw]

Originally Posted by jovica

Hi Bill,

I have a measure function (button) but i'm not sure what for(i believe it's for tool geometry offset). When i press it, it says "Key no data"(something like that )

For turning tools: T11, T12, T13, T14, T15, T16
For milling tools: T21, T22, T23, T24, T25, T26
Offset for them: Because tool is called with T1101, these two last numbers are offset, i think offset is unique for all of them. I just need to be careful not to mix them. I can't use tool offset 33 for T12 and T13, if you know what i mean.

My way:
I choose a tool let's say T1233. G54 is set to 0,0,0,0. My tool geometry offset (No. 33) is X0,Y0,Z0,R0,Q0. Now when i start my program( i think it goes from machine zero G28 U0. G28V0. G28) i see how much i need to add (+-) in that tool offset to get to the top of my work piece. And somehow it works.

It is too slow. If i have G54 in program it's useless. I thought i can set G54 offset and tool offset like in HaaS VF4 with 3D taster. I know that this Fanuc is an old machine but i believe there is faster way to do this, somehow.

Regardss,
Jovica

Hi Jovica,

With regards the Measure Function, you have to write a value before you press Measure. The Measure feature can work in a number of ways, it was up to the MTB as to how this feature was organized. Some have a Setting value set in parameters that is used in calculating how far the tool tip is from from a fixed feature of the machine, others simply use the distance the tool is from X, Y, Z Machine Zero (Zero Return Position).

Lets say that you're setting the Z Offset for T1101 (Offset 01)
1. You pick a surface of the machine that will stay constant, and can be reached by the tool. The face of the chuck for example.
2. Index T1100 into position
3. Move the tool down to touch either a dial indicator type, or LED type setting gauge, or a setting block that will be reserved for this purpose. You don't want to actually touch the face of the chuck as you will end up marking it.
4. Select the Offset Page containing Offset 01 and place the cursor on the 01 Offset Line. Key in Z0, and Press the Soft Key [MEASURE]. The value in Z for Offset 01 should change. Now, depending on whether there is a value set in parameters for the Measure function, will determine what value is stored. I don't know what parameter that will be for your machine; you will have to find that from the manuals you have.
5. Take a look at the current Machine Position value for Z, if the value stored in Z for Offset 01 is the same as the machine position, no value is stored in parameter.

I have only given the above explanation to indicate how the Measure Feature is used. The above method, if no value is set in parameter, will store the Air Gap between the Tool Tip, when the Tool is at Zero Return, and the Setting Gauge. I don't particularly like that system and I can show you another method that is used by the majority of CNC shop. This method conveniently lends itself to setting tools, particularly the milling tools, away from the machine.


Look at the pictures above. If you want this method described and implemented, get the measurements asked for in the two pictures.

1. The vertical Z dimension shown in the Left picture is from one of the faces of the outside hexagonal form of the turret to the face of the Chuck. The X dimension is from Tool Spindle centre line to Chuck centre line. Two more dimensions are require and are not show in the picture, to have draw them in may have confused the issue. These two dimensions are from the centre line of the Tool Spindle to the centre line of the Chuck in the Y axis, and from the Front face of the turret to the Chuck centre line in Y.
2. The vertical Z dimension shown in the Right picture is from the Tool Spindle centre line to the face of the Chuck. The X dimension is from one of the faces of the outside hexagonal form of the turret to Chuck centre line. The Y dimensions not shown, will be the same as in the Left picture, so you wont have to get these again.
3. All dimensions are measured from the Zero Return Position for X, Y and Z.
4. The Machine Position Display should read Zero in all axes when the slides are at Zero Return. Accordingly, you can use the Machine Position Display to give you the required dimensions. You use the machine as a measuring machine.

If you wish to go further with this, Post the dimensions and I'll write the Macro Program for you.

Regards,

Bill

[jovica]

Hi Bill,
I will try this method with measure button and i'm also interested in your another method.
And what about G54-G59? Are you going to use them in your macro program?
I have this image (in attachment) for measurements. Can it help?
In your macro program can i change these measurements? They are in variables?

Regards,
Jovica

[angelw]

Originally Posted by jovica

Hi Bill,
I will try this method with measure button and i'm also interested in your another method.
And what about G54-G59? Are you going to use them in your macro program?
I have this image (in attachment) for measurements. Can it help?
In your macro program can i change these measurements? They are in variables?

Regards,
Jovica

Hi Jovica,
There will be a Macro Program for Tool Setting and for Work Shift, G54 to G59.

When the milling tools are used in the horizontal plane, do they use the same Tool Number as when indexed to the vertical plane? Please explain the use of Tool Numbers in the two different aspects.

The Drawing helps but you still need to accurately measure the features I've specified. The drawings are only Ball Park dimensions, the actual dimensions can be altered by parameter just by moving the Zero Return Position. The dimension I've specified are not hard to get accurately. For example, to get the dimension of a Milling Spindle centre from X and Y Zero Return to Centre of "C" axis, just dial in the Spindle over the "C" axis. When Zero all round with a dial indicator, look at the X, Y value in the Machine Position Display. The values that you see represent the distance and direction from Zero Return for X and Y.

Regards,

Bill

[jovica]

Hi Bill,

I know that you need accurate measures but that machine is in other town so i only have that drawing and that is the reason why i asked you if i can change that dimension in macro variable.

Now the tool numbers. Yes, they use the same Tool Number but i only worked with turning tools because i need to do a turning operation. Maybe later some milling operation. When i call some tool he rotates and stops vertical on "C".

Regards,
Jovica

[angelw]

Originally Posted by jovica

Hi Bill,

I know that you need accurate measures but that machine is in other town so i only have that drawing and that is the reason why i asked you if i can change that dimension in macro variable.

Now the tool numbers. Yes, they use the same Tool Number but i only worked with turning tools because i need to do a turning operation. Maybe later some milling operation. When i call some tool he rotates and stops vertical on "C".

Regards,
Jovica

Hi Jovica,
I'll write the Macro programs using dummy values for the indicated dimensions in my previous Posts. You can then replace these with real values when you determine them. In actual fact, you can use incorrect values, so long as you always use those values. If someone ever changes the values and doesn't correctly reset ALL previously set Tool Offsets, then you will have problems.

Have you used the milling feature on your machine before? Are there any example programs in the manual showing milling tools being used in the Vertical and Horizontal plane that you can Post here, or send to me?

When using the same milling tools is the Horizontal plane as used in the Vetical, the length of the tool will have to be accommodated in the X axis instead of the Z axis. Is there any axis swapping going on to achieve that, or is a different Work Shift used?

Regards,

Bill

[jovica]

Hi Bill,

Ok, i will replace them with real values.

I didn't use milling features at all. Primary task is turning. Someone wrote this program (old.txt) but i never used it. I tried S1000 M04 for milling tool just to see that everything works.

This machine will work 3 or 4 turning features(products), that is if i accomplish to setup it, and then some milling features.

Regard,

Jovica

[angelw]

Originally Posted by jovica

Hi Bill,

Ok, i will replace them with real values.

I didn't use milling features at all. Primary task is turning. Someone wrote this program (old.txt) but i never used it. I tried S1000 M04 for milling tool just to see that everything works.

This machine will work 3 or 4 turning features(products), that is if i accomplish to setup it, and then some milling features.

Regard,

Jovica

Hi Jovica,
Just a couple more questions.

1. You said that when using a milling tool in either the horizontal or vertical plane, the same tool number applies. If for example T2121 is called, how does the control know to use it in the Horizontal or Vertical plane? Is there an M code or other code that forces the same tool number to index to either the Horizontal or Vertical plane?

2. Do you use the Turning/boring tools only in the Vertical plane?

Regards,

Bill

[jovica]

Hi Bill,

In program i call T2201 but i'm working with tool offset T2101. This way tool T21 is in horizontal plane.

Yes, i only use Turning/Boring in vertical plain.

Regards,

Jovica

[angelw]

Originally Posted by jovica

Hi Bill,

In program i call T2201 but i'm working with tool offset T2101. This way tool T21 is in horizontal plane.

Yes, i only use Turning/Boring in vertical plain.

Regards,

Jovica

Hi Jovica,

In one of your previous Posts, you state "M55 for turning (C axis)" In the file old.txt you attached in an earlier Post, it has the following block:
M55(LINKE DREHSPINDEL ANWAEHLEN). This means left hand turning spindle selected. How does that comment relate to "M55 for turning (C axis)" What is M54?

I've had a look at the old.txt program, and it seems that different Work Shifts are used to accommodate tools in different planes. This what I expected unless there had been an axis swapping command.

You will have to look up in your Fanuc manual to see which System Parameters are used for Tool Geometry Offsets. With a conventional Turning Centre #2001 to #2064 are used for X Tool Wear Offsets 1 to 64. In a Machining Centre, #2001 to #2200 are used for the Geometry Length Offset of the Milling Tool. So the question to you is, does your machine use Turning Centre System Variables to set the Geometry Length Offset for Milling Tools?

Try the MEASURE function to set the X Geometry for a Turning Tool. Do as follows:
1. Call the Tool to be measured into the spindle.
2. Place a short piece of material in the chuck so to be able to turn a diameter on it.
3. Turn a diameter long enough to measure with a micrometer.
4. Clear the tool of the turned diameter in the Z axis only. Do not move the tool in X.
5. Stop the spindle and Measure the diameter.
6. Select the Offset Page and place the cursor on the X Geometry Offset of the Offset to be set.
7. Key in the Measured diameter and press MEASURE.

Post back the result of the above.

Regards,

Bill

[jovica]

Hi Bill,
That is interesting. I can't tell you exactly. When i run M55 in MDI mode a turning lamp on the main panel is on. Then M54 is milling lamp.

Here are the list of M-code:
00 Program stop
01 Optional program stop
02 End of program
03 Main spindle start (CW)
04 Main spindle start (CCW)
03 Milling spindle start (CW)
04 Milling spindle start (CCW)
05 Main spindle/Milling spindle stop
08 Coolant ON
09 Coolant, Air OFF
10 Chuck clamp
11 Chuck unclamp
19 Spindle orientation
30 End of tape
46 Automatic door open
47 Automatic door close
48 Chamfering effective
49 Chamfering ineffective
52 Spindle (C-axis) lock ON
53 Spindle (C-axis) lock OFF
54 C-axis gear ON
55 C-axis gear OFF
98 Calling of subprogram
99 End of subprogram

Ok, i'll wait for you post.

Regards,
Jovica

[angelw]

Hi Jovica,
I haven't forgotten about the setting Macro programs. I'm having trouble getting my head around how the milling tools are used in the Horizontal plane.

I understand that you call up whatever tool in the Vertical spindle, using a different Tool Offset Number, to have the desired tool in the Horizontal plane, but that doesn't explain how the Tool Length is accommodated. I know you could use a different Work Shift Offset with modified X and Z vlaues, but that would require a different Work Shift Offset for every tool used Horizontally in the program. To me that seems really clumsy and fairly ordinary in terms of the MTB, and I'm surprised that there would not be another method. Is there no mention in the manual of any axis rotation when using tools in the Horizontal plane?

Regards,

Bill

[jovica]

Hi Bill,

I was pretty busy these days. Thank you for your help, machine works on my way. It is strange but it works. I need to write programs manually, post processor is not working. I will write you another post later for tools, measure...

Best regards,
Jovica

[jovica]

Hi Bill,

To continue from my last post.
I told you that this machine need to do 2 or 3 products. So i needed a solution for them. With your help i managed to do these products.

Now i'm using Tool offset from machine zero, G54-G59 and tool wear. Although i need to manually set and correct them it's working My post processor is good but it needs some corrections.

Thank you for your time.

Regards,
Jovica