[REVCAM_Bob]

In our wire machine there is a parameter number 15201 , (this is an 18i ontrol
on a fanuc wire edm).

The parameter controls the reverse alarm distance. i.e. if the wire shorts out
the machine will attempt to move backwards to clear the short and then start
cutting again. If it moves beyond the distance specified in this parameter,
the machine will alarm out..

I need to be able to change the parameter from within a program.

Does anyone know how to do this?

Thanks again, you guys are great!

[REVCAM_Bob]

This looks like a pretty good site for some variable... I mean valuable tips!!:rainfro:

allows parameter change from within a program...


http://www.machinetoolhelp.com/Appli...statement.html

[REVCAM_Bob]

the above just errored out G10L50 stuff.....

Any one have any other ideas how to set parameter values from within a program?

[dcoupar]

Bob,

Perhaps if you posted what your program looks like, and the alarm number?

According to the manual I have, it appears as if this should work:

G10L50
N15201 R1000
G11

Dave

[gar]

070121-1427 EST USA

REVCAM Bob:

On a HAAS machine, these are similar to Fanuc, many parameters can be directly changed thru an associated #number variable. In HAAS this requires MACROS.

If your 15201 is actually the numeric part of a #number address, then you could do
#15201 = 2.345 or what ever
and assuming it can be changed at any time.

If not there may be some other #number address associated with this parameter.

In a few cases in HAAS changing a variable does not take immeadiate effect.

.

[REVCAM_Bob]

I tried all of the following:

G10L50
N15201 R30000
G11
==> 003 Alarm: Value exceeding maximum number of character was detected.


;then
G10L50
N15201 R00030000
G11
==> 003 Alarm: Value exceeding maximum number of character was detected.


;then
G10L50
N15201 R00030000
==> 003 Alarm: Value exceeding maximum number of character was detected.



;then
G10L50
==> 110 Alarm: Absolute value of fixed point representation exceeds allowable range.



;then
N15201 R00030000
==> 003 Alarm: Value exceeding maximum number of character was detected.


Maybe it thinks it is a line number.... ??

%
N1 O1(9 MINUTES)
N2 (R1TAB1S2S)
N3 M31 (MACHINING TIMER RESET)
N4 M15 P0 (VERTICAL CUTTING)
N5 G90 (ABSOLUTE POSITIONING)
N6 G10 P1 B0 (DO NOT SKIP LINE /1)
N7 G10 P2 B0 (DO NOT SKIP LINE /2)
N8 G10 P3 B1 (SKIP LINE /3)
N9 G10 P4 B1 (SKIP LINE /4)

N10 M45
N11 G53 Z-1.0
N12 G53 X-10.85974 Y-14.40714 (PALLET 12)
N13 G93 X0 Y0
N14 G92 X0 Y0

N15 (EDM3 A2/D2 1.500 123STRAIGHT)
N16 G10 P1 R0.00782 (REDUCED 0.0002)
N17 G10 P2 R0.00547
N18 G10 P3 R0.00515
N19 G10 P10 R0.00588

G10 L50
N15201R00030000
G11


N20 G10P1(A2/D2 1.500 123STRAIGHT)K1X11Y4Z31U6V140W23I13J6A130C10E13Q0L1 65
N21 G11P1Y12X1Z1U500V3W2
N22 G10P2(A2/D2 1.500 123STRAIGHT)K2X11Y6Z6U2V90W64I2J0A170C13E6Q0L362
N23 G11P2Y12X1Z1U1000V1W2
N24 G10P3(A2/D2 1.500 123STRAIGHT)K3X12Y8Z0U2V80W30I0J0A170C13E4Q1L441
N25 G11P3Y3X1Z1U1000V0W2
N26 G10P20(REDUCED FLOW)K1X11Y4Z31U6V140W23I13J6A130C10E4Q0L165
N27 G11P20Y12X1Z1U500V3W2
N28 G10 P9998 R0.0000 (CLEARANCE)
N29 #101=#5023
N30 #103=#5024
N31 #102=#101+0.00000
N32 #104=#103+0.00000

etc....................

[REVCAM_Bob]

I tried #15201=5000 and it also caused an alarm ;(

[dpuch]

First find out what the current value is in N15201 then try changing it by -1 to see if it works.
With fanuc macros enabled you can MDI
#15201=#15201-1;

Otherwise something like what you tried earlier, but try a smaller number...
G10L50
N15201 R30
G11

The error ==> 003 Alarm: Value exceeding maximum number of character was detected.
looks like your just trying to put too large a number in. You would have to check the manual for the max value allowed.

Dale

[Dan Fritz]

I've never heard of a method for changing parameters from a program on a Fanuc. If there is such a feature, it's not documented.

[dpuch]

Changing variables is well documented under custom macros.
Note the system variables 1000+

See the page from the fanuc 16i manual attached.

[codyst]

If the parameter number you are changing controls more than one axis, you have to specify the axis number you want to change.

G10L50 (programable parameter entry ON)
N15201 P Axis number R setting value (1=X, 2=Y, 3=Z...etc)
G11 (programmable paremeter entry OFF)

Also, some values can not be changed with a G10 statement due to the way the software controls that action. If you change it from the parameter screen and it throws an alarm for power down, you obviously won't be able to change it in cycle. If you are putting a decimal point in the setting value, it won't like it either.

I've never heard of a method for changing parameters from a program on a Fanuc. If there is such a feature, it's not documented.

It's documented, just not very well, as it's not recommended.

[Dan Fritz]

codyst: Thanks for the tip. I stand corrected.

[REVCAM_Bob]

The documented part appears to be for macro variable, but not parameters....
Still will be trying today though!!

[dpuch]

The documented part appears to be for macro variable, but not parameters....
Still will be trying today though!!

You are correct, I just looked over it again and realized I was lumping the system variables and system paramaters together.

[dpuch]

Well one way to get the proper format might be to punch out your parameters. Look at the line for the parameter you want in the file and use that format.

Besides having a backup of the parameters is a good thing.

Dale

[REVCAM_Bob]

How do you punch out parameters??

[Al_The_Man]

Set up your PC to save, Go to EDIT mode press the dgnos/param, parameters and then output/start key
If you want to output the 900 parameters also, press and hold the EOB key when pressing output/start.
Al.

[Camtomeron]

G10 is, in fact, the way to set parameters programmatically. It is the only way. The alarm is raised by the value passed. Try a smaller value. This value should be related to the stroke limit value. Consult your Fanuc parameter manual for parameter info, the Fanuc operation manual for G10 instructions, and your MTB (machine tool builder) manual for the stroke limits if unknown to you. Good luck.

[debco99]

I was chatting with Dick Swisher at GE Fanuc today and asked him about your problem.

He was aware of exactly what you need to do, it requires an option to be used with the G10.

Give him a call at 1-800-GEFanuc .

Good Luck

[REVCAM_Bob]

Does Dick Swisher have a direct line. I got put into a general pool and don't know who I will end up talking to...