[hmc710]

Hi All,
Finally put power on the old Acroloc M15 we picked up a while back. Powered up and everything seems ok. Its got the Faunc GN11M control with the associated years of grime and coolant on the panel face and sticky buttons. What's the best way to clean these and free up the sticky buttons? This is an old tape machine but I am pretty sure the prev owner had it hooked up to serial cable. Is there a program line limit on this machine like our TNC145 1000 line limit?
Thanks,
H

[angelw]

Hi All,
Finally put power on the old Acroloc M15 we picked up a while back. Powered up and everything seems ok. Its got the Faunc GN11M control with the associated years of grime and coolant on the panel face and sticky buttons. What's the best way to clean these and free up the sticky buttons? This is an old tape machine but I am pretty sure the prev owner had it hooked up to serial cable. Is there a program line limit on this machine like our TNC145 1000 line limit?
Thanks,
H

I haven't seen GN in the specifications of a Fanuc 11 series control before, so I'm assuming its just an 11M with a CRT screen. This being the case, the machine control is a CNC with a Tape Reader, and is more than just an old Tape machine. If this is all correct, then the number of lines is limited only by the memory size of the control. If the control has a RS232 interface, any program too large to be loaded in the memory can be drip fed to the control from a PC using Tape Mode set at the control.

Regards,

Bill

[hmc710]

It is a General Numeric 11M and the CRT and controls in back all say Fanuc. I have read its the same as a Fanuc 6M and it does reference that in the workbook. Not a real control manual, just a quick example book. What is the best way to clean the keypad?
THanks,
H

[angelw]

It is a General Numeric 11M and the CRT and controls in back all say Fanuc. I have read its the same as a Fanuc 6M and it does reference that in the workbook. Not a real control manual, just a quick example book. What is the best way to clean the keypad?
THanks,
H

What I said in my last post will apply, the number of lines is limited only by the memory size of the machine. The fewer number of commands and therefore bytes, in each line, the greater number of lines will the controller accommodate.

To limit the amount of memory consumed by the program, and therefore allow longer programs to be loaded into memory, leading zeros can be dropped and modal commands eliminated. For example the following commands on the left can be written as they appear on the right:
G00 = G0
G01 = G1
G02 = G2
G03 = G3
G04 = G4
M00 = M0
M01 = M1
M02 = M2
M03 = M3
M04 = M4
M05 = M5
T01 = T1

Further, if a preceding command is a modal command, it can be dropped until its canceled by another modal command from the same group. For example, the following blocks are all equal in meaning:

G1 X100.25 Y25.5-------------G1 X100.25 Y25.5
G1 X120.25 Y25.5-------------X120.25
G1 X120.25 Y125.5------------Y125.5
G1 X100.25 Y125.5------------X100.25
G1 X100.25 Y25.5-------------Y25.5

Sequence numbers are not required on each and every line. Many only put a sequence number on the first line of each new tool, so that if a restart is required, searching for the start of the information for that tool is simple; you just search for the sequence number for that tool.

If you have the control connected to a PC, or some other external I/O device, you can be more verbose with how you write your programs, that is, include the modal coordinates as shown in the program example shown in the left hand column above, by saving your programs on the external device and only loading the program being currently used. I prefer to do it that way, as for me, the programs are more readable.

Your control will have a Tape mode, and therefore, programs that are too large for the machine's memory can be run in a DNC session from the PC via the RS232 interface.

Regards,

Bill

[hmc710]

Thanks Bill,
I've been working on my G code skills on the Fanuc OT lathe control. I do tend to "over write" my programs, just for follow up or editing at a later time. Any ideas what the cable and baud rate settings might be on this machine? I have read on other posts about saving the parameters to tape. I would assume this could be done also via RS 232 but I have not found any mention of that in the workbook yet. Someone had mentioned 6M manuals are available from Fanuc at a reasonable price.
Thanks,
H

Just found the General Numeric control maintenance manual in a box of parts...... no operations manual yet...

[angelw]

Thanks Bill,
I've been working on my G code skills on the Fanuc OT lathe control. I do tend to "over write" my programs, just for follow up or editing at a later time. Any ideas what the cable and baud rate settings might be on this machine? I have read on other posts about saving the parameters to tape. I would assume this could be done also via RS 232 but I have not found any mention of that in the workbook yet. Someone had mentioned 6M manuals are available from Fanuc at a reasonable price.
Thanks,
H

Yes, you will be able to save the machine's parameters to an external I/O device, such as a PC, via the RS232 interface.

1. Connect the external I/O device with the I/O interface.
2. Select EDIT MODE on the control
3. Press the 'SERVICE' software key followed by the 'PARAM' software key to select the Parameter screen.
4. Press the 'PUNCH' software key followed by the 'PARAM' software key and all the parameters, except the pitch error compensation data, are punched.
5. The procedure for punching pitch error data is similar except that the 'PITCH' software key is pressed where the 'PARAM' software key was pressed in 3 and 4 above.

You should find a DB25 female connector somewhere on the machine; this is the RS232 interface to an external I/O device, often a PC. The cable configuration is as follows:

Use shielded cable with at least 3 insulated wires, and a bare wire trace. Shielding means that the signal wires are wrapped in either a fine copper wire mesh, or more commonly, aluminum foil. The bare wire trace is an uninsulated wire running full length of the cable and obviously, in full contact with the shield. This is the wire that's connected to pin 1 on the machine end.

Regards,

Bill

Machine End-------------------PC End
DB25 Male-----------DB25 Female-----DB9 Female
1---Shield-----------N/Connected-----N/Connected
2-----------------------3----------------2
3-----------------------2----------------3
4
| bridged
5
7-----------------------7----------------5
6
|
8 all bridged
|
20

To set the following parameters, in MDI mode, go to the Handy parameters and set the PWE bit of parameter 8000 to one. The machine will go into Alarm mode 100; this is normal. When finished setting the parameters set 8000 back to off (zero) and hit Reset to eliminate the alarm condition.

Set the following parameters
#0000
TVC = 0
CTV = 1
ISP = 0
NCR = 0 This will depend on your PC software. 0 = LF, CR, CR 1 = LF
EIA = 0

#0020 = 1
#0021 = 1
#0022 = 1
#0023 = 1
#5001 = 3
#5110 = 3
#5111 = 2
#5112 = Baud Rate (10 = 4800) starting point

Setting for the Setting Page
I/O = 1
ISO Format = 1

You need software installed on the PC to transfer data to and from the machine. The communication settings of the transfer software should be set as follows:

Baud Rate = 4800 (starting point)
Data Bits = 7
Stop Bits = 2
Parity Bit = even
Handshake Mode = Xon Xoff (also known as software handshaking)

[hmc710]

Thanks,
Will give this a try when I get a chance.
H

[hmc710]

Will try using my Bobcad to com with the mach and see what happens. On my keypad screen the #9 does not seem to work. Is there a way to check this? The machine is an Acroloc M15 with the tool changer. In the work book it talks about using the M19 command, spindle stop & orientate, prior to raising the spindle and I can't get any command with a 9 in it to work. When I jog Z down it does pick up a tool and it orientates it back on the way up. Is the M19 used before every tool change?
Also paging through existing programs; On my OT control you enter the Oxxxx program number and arrow down key and it loads the program. The work book does not say how to load an existing program from memory. Tried input, arrow keys, etc and it stays on the same program. Any help here?
Thanks,
H

[angelw]

Will try using my Bobcad to com with the mach and see what happens. On my keypad screen the #9 does not seem to work. Is there a way to check this? The machine is an Acroloc M15 with the tool changer. In the work book it talks about using the M19 command, spindle stop & orientate, prior to raising the spindle and I can't get any command with a 9 in it to work. When I jog Z down it does pick up a tool and it orientates it back on the way up. Is the M19 used before every tool change?
Also paging through existing programs; On my OT control you enter the Oxxxx program number and arrow down key and it loads the program. The work book does not say how to load an existing program from memory. Tried input, arrow keys, etc and it stays on the same program. Any help here?
Thanks,
H

You stated that the machine was fairly dirty, you could give the whole key pad arrangement a clean. Carefully unplug it from the control to do the best job. Examine the area associated with the 9 button to see if there are any signs of damage or sticking. I haven't handled one of these for a long time, but you can probably check the function with a multi-meter. Trace the circuit to were it connects to the machine and apply the test there. Check the result against a working key for a comparison so that you know your test is viable.

A work around until you fix it, get it fixed, or get a replacement, is to write and edit your programs on a PC and upload them from there.

Explain more about the mechanics of the tool changer. I don't understand your meaning of "When I jog Z down it does pick up a tool and it orientates it back on the way up". That seems to me that you're saying that the spindle orientates after the tool has been picked up.

The idea behind orientating the spindle for tool changing, is to do it prior to picking the tool up so that the drive dogs of on the spindle nose are aligned with the corresponding cutouts in the tool holder. If this is not done, and the drive dogs are misaligned, then these dogs will interfere with the tool changer ring on the tool holder. Accordingly, the spindle must be stopped and orientated prior to doing a tool change. Most controls combine the M19 function into a tool change routine, which is either executed through the PMC, or via a USER MACRO program, yet some machines had to have the M19 included in the program prior to the tool change. If your machine is in the latter group, and your control has the USER MACRO option, then a MACRO program can be written to include the M19, and called by M06. This way you will only have to program the tool number and the M06 to carry out a tool change.

Check to see if your control has the User Macro option. In MDI, input the #1=1 and execute the command to see if the control accepts it. If it does then your control will probably have the option. Check that the value of Macro Variable #1 is 1 by navigating to the MACRO SETTING page. There are a few different versions of the 10M control, the most noticeable difference is a version with a 9" screen verses one with a 14" screen. The functionality of the two are similar, but the soft key layout is a little different.

To go to the MACRO SETTING page:
1. Press the function key at the bottom left of the screen
2. Press SETTING repeatedly until the MACRO setting page appears
or
3. Press SETTING, press CHAPTER, and a set of soft keys will appear at the bottom of the screen, one of which will be labeled MACRO
4. Press MACRO

If you have a MACRO setting page then your machine will have the USER MACRO option.

Go to the local variable listing and check the value of #1. It should be 1.

To call a program that is already registered in memory:

1. Select Memory or Edit mode
2. Press the Function Menu key.
3. Press PROGRAM key; program text is displayed on the screen.
4. When program text is not displayed:
i. Press the CHAPTER key to change over the soft key to the chapter
selection key and press the TEXT key.
or
ii. Press the PROGRAM key repeatedly until the program text is displayed.
5. Press operation menu key to change over the soft key to operation selection key.
6. Press FW-SRCH (FORE SEARCH) key.
7. Press PRO# key, "O" is input into the input buffer and the operator is prompted to enter the program number to be searched.
8. Enter the program number and press EXEC.

If the program exists, it will be loaded for use.

It sounds long winded, but its fairly quick and easy once you've done it a few times.

Regards,

Bill

[underthetire]

Acrolocks used a funny holder, at least the old dogs I have seen. They didn't orient the spindle, just had a slow jog to get it to snap in if I remember correctly. Those machines were older than this one though.

[hmc710]

Thanks Guys!
Bill, I am copy & pasting your comments, thanks.
On start up, I jog away from axis zero's then select Zero Return and use +Y, +Z, -X to "reference or zero" all axis. The work book said I can't use the MDI function until the machine does this. When I jog -Z down it takes the tool in line with the spindle with it. This is a 15 tool carousel and the tool used or called is always directly under the spindle. When the spindle advances -Z the tool holder snaps into place on the end of the spindle. When the spindle retracts (as in Zero Return) it slows down at the carousel, rotates automatically (orientates) and then unsnaps from the spindle as the spindle contiues up to Zero. The work book says to use M19 to stop and orientate the spindle "M-15: Because of the spindle orient feature of the m-15, the z axis zero return must be made in the orient position to insure that the tool holders are depositied in the disc with their drive pins position in the alignment with the groove or track cut into the uderside of the top of the tool disc. Spindle orientation is automatic only when the spindle is turning during zero return. if the spindle is to be retracted by zero return when it is not turning, the move should be prededed by a MDI command M19 (stop & orientate). The spindle should be turning when the M19 command is given."
So it says its automatic when its turning. I just went out and jog -Z w/spindle off, picked up the tool, jog +Z and at around 2" it orientates back and forth and drops the tool, contiues back up. I did a G00Z-4.5S500M03EOB input start and it picks up the tool and the spindle starts. Before when I tried to Move +Z it got to the orient location and alarmed out with Orient Plunger not engaged . I just tried again without a M05 command. The spindle stops when it gets close then alarms with the Orient Plunger fault. So that tells me it needs the M19 so it looks like I'll find out what the inside of the control looks like.
Thanks guys.
H

[Indmach]

I have acroloc M15 machine
you have to do it
G28 Z1.00 and it will go home
Than call tool
T12 or what ever you need
m19 doesn't work on these old machine and
if your spindle is not oriendtating go on the top of the Z axis you will see a attachement attached to your spindle with some proxy switches take that attachment off.
there is a solonoid valve it needs cleaning because it work with spring loaded cylyinder there is a seal in it and it might need cleaning or not going into the Z azis to push the spindle to its position. Becuse there is a cutout on your spindle on the top that cylinder goes and push that cut out to the desired location and it always goes not same position. If you are not orientaing your spindle you will hear a big noise coming out from the top very soon because that valve is not going back and its been pushed by your spindle and it make nasty noise like some thing is broken inside I was ****ting in my pants when it happnes to me.
if you want I can send you some pics/
Regards
Ron

[Indmach]

Fanuc 11 control
When I turn on the machine it does not show the screen numbers but it show a horzotical lines but If I wait and shut the machine couple of times than its fine what it could be screen or control problem.
Please help
Ron

[angelw]

I have acroloc M15 machine
you have to do it
G28 Z1.00 and it will go home
Regards
Ron

The command G28 is Reference Return through an intermediate point. Accordingly, you have to be a bit careful how its implemented. Its a two shot command and this aspect can be observed in single block mode. When G28 is executed in single block, the cycle start has to be pressed twice to have the slide return to the machine zero point; once for the slide to go to the intermediate point, then again to have it complete the Reference Return.

If the control was in absolute mode when the G28 is executed, the slide would move at rapid speed to the coordinate programmed with the G28, then go directly to the Reference Return position. If the control was in absolute mode (G90) and the slide sitting at Z200.00mm when G28 Z1.00 was executed, the slide would rapid in a Z minus direction, 199.00mm. If there happened to be anything in the way, then you have a crash on your hands. Therefore, its a good idea to program G28 in incremental mode and with a value of zero as in the following example:

G91 G28 Z0.0. This command effectively tells the control to Reference Return through an intermediate position Zero distance away from the current position.

Regards,

Bill

[hmc710]

Thanks Guys,
Will digest this and give it a try. I want to look through the other programs and see if I can tell how they have been programmed for these actions. I have not had a chance to try to pull up other programs or see if I am Macro compatable yet. The machine is in incremental mode right now.
Also: I have a 4th axis for the machine. It looks like it just plugs into a connector on the frame. Is it Plug and Play, will the control recognize it, or will it have to be configured when hooked up?
Thanks for all the help!
H

[angelw]

Thanks Guys,
Will digest this and give it a try. I want to look through the other programs and see if I can tell how they have been programmed for these actions. I have not had a chance to try to pull up other programs or see if I am Macro compatable yet. The machine is in incremental mode right now.
Also: I have a 4th axis for the machine. It looks like it just plugs into a connector on the frame. Is it Plug and Play, will the control recognize it, or will it have to be configured when hooked up?
Thanks for all the help!
H

Unless the 4th axis came with the machine, I guarantee that it won't be Plug and Play. Check in the control cabinet for a start to see if it has a 4th axis servo amplifier fitted. I've seen many machines with connector in place and some of the wiring loom, but no drive. There are parameters to set to enable the axis.

Regards,

Bill

[hmc710]

There were 4 running machines that came from a local co. and I believe the guys said they all had the 4th axix on them. I've got a couple sitting here so will see if one is marked for this machine.
H

[hmc710]

The current program in the machine starts with
N1;
T15 G90 G20 G54 G00 Xxx Yyy S3000 M3;
G43 H15 Z.1 M08;
G04 P500;
G81 G99 R.1 Z-.35 F5
G80 G28 G49 Z0;
N2;
T3 G90 G20 G54 ....

Assume machined was zero to start. Select tool 15 absolute mode. Don't have a listing for G20. G54 is a work offset I think, run spindle at 3000 rpm.
G43 initiatesTool Offset H15, move to Z.1, coolant on. G04 dwell.
G81 canned drill cycle
G28 Ref Return G49 cancel Tool Offset, goto Z 0.00" (machine zero)
T3 pick up new tool.

You kind of lost me on the "its a good idea to program G28 in incremental mode with a value of zero. Ex: G91 (inc) (G28 Ref Return) Z0.0 (no inc movement)"
Thanks,
H















Tool 15 Absolute mode G20? G54 Work offset? Spindle 3000 rpm Spindle on

[angelw]

The current program in the machine starts with
N1;
T15 G90 G20 G54 G00 Xxx Yyy S3000 M3;
G43 H15 Z.1 M08;
G04 P500;
G81 G99 R.1 Z-.35 F5
G80 G28 G49 Z0;
N2;
T3 G90 G20 G54 ....

Assume machined was zero to start. Select tool 15 absolute mode. Don't have a listing for G20. G54 is a work offset I think, run spindle at 3000 rpm.
G43 initiatesTool Offset H15, move to Z.1, coolant on. G04 dwell.
G81 canned drill cycle
G28 Ref Return G49 cancel Tool Offset, goto Z 0.00" (machine zero)
T3 pick up new tool.

You kind of lost me on the "its a good idea to program G28 in incremental mode with a value of zero. Ex: G91 (inc) (G28 Ref Return) Z0.0 (no inc movement)"
Thanks,
H
Tool 15 Absolute mode G20? G54 Work offset? Spindle 3000 rpm Spindle on

G20 selects Imperial Mode, G21 Metric. G54 is a work offset; you should have G54 to G59 available.

G28 is Reference Return through an intermediate point. You can use it in absolute mode, but you have to plan the intermediate point, you just can't expect that the slide will return directly to the Reference Point. In the example of using G28 Z1.00, you would have to be careful of the current absolute position of the tool if the G28 command was made in absolute mode. If the tool was at Z0.00, then no problem, the tool would make a positive move of 1.00" to return to the Reference point through Z1.00. If the tool was at Z6.00 with the same G28 Z1.00 command, the tool would move Z minus 5.00", then in a positive direction to the Z Reference position. If G28 is executed in incremental mode and with a Z value of zero, the slide will return to the Reference point directly, no potential surprise move.

Its common for a tool change to take place at either the G28, Reference Return position, or at Second Reference (G30) point if the machine has that option. If the T command in your example program initiates a tool change, I would bet that there is a User Macro program that's called by a T command, and includes a G28 command.

Regards,

Bill

[hmc710]

In the programs I have called up so far (Search Fwd - Next Program) the tool changes are like the example, the Cancel the tool offset then G28 and a Z 0
I'll look around at your example of the Macro and see what I can find.
Thanks a lot!
H