[adaptaflex]

Hi All

Has anyone got any suggestions ?

We currently use a set of logic so that we can increase the speed of turning and boring operations as we progress along a bar length (we can spin a short bar faster than a long bar).

We have used the code below successfully on our Mori Seiki SL25 that has a Fanuc 10T controller. When we tried the same code on another SL25 but with a Fanuc 10TF controller it would not recognise the code….eg it converts the IF command to I F (I space F).
The code we use is as below.

(#500 = Part counter)
(#501 = Set speed)

N101 (Decide which speed to use)
IF[#500LT15]GOTO102 (Slow speed)
IF[#500LT20]GOTO103 (Low speed)
IF[#500LT30]GOTO104 (Medium speed)
IF[#500LT71]GOTO105 (High speed)
(If count is equal to 71 then bar is finished)
#500=0 (Reset counter)
GOTO101

N102 (Set Slow speed)
#501=1650
GOTO107

N103 (Set Low speed)
#501=2000
GOTO107

N104 (Set Medium speed)
#501=2250
GOTO107

N105 (Set High speed)
#501=2500
GOTO107

N107 (Increment counter and start cutting program)
#500=#500+1

(Cutting program)
G97S#501M03
G0T0202M08


M03
G97G0S#501T0202M08

PS Please be gentle with me I am not a CNC expert this code was adapted after being kindly submitted by this forum

Thanks Guys
Mark

[Sump Cleaner]

Mark,

Does your control have macro B enabled? Is sounds like it is not and the controller is taking IF as an I value and a F value.

JK

[Al_The_Man]

Check to see if parameter 9111 bit#0 is a 1.
Al.

[adaptaflex]

Thanks Guys
Most helpful as always!

Mark

[adaptaflex]

Hi
I have tried changing parameter 9111 bit 0 to 1 the return message is "locked Parameter"
I have also set the PWE bit of parameter 8000 to 1 but this makes no change.
Do I need to power down then up after setting the pwe bit?

Regards
Mark

[Al_The_Man]

IIRC this is normal see attached for loading by PC.
Al.

[adaptaflex]

Thanks Al
I am still getting a locked parameter message I am loading this from the machine keypad ....does that make a difference?

[rajesh_1355]

You will hve to initialize the system for changing the option bit. Mean deleting all the data then loading option bit then a data loading special procedure. Take help from Fanuc.

[hollycncsimmo]

Thanks Al
I am still getting a locked parameter message I am loading this from the machine keypad ....does that make a difference?

Have you manage to enable Macro B yet? If not i can help but 1st make a notes of your PMC lists,you will find them after you press NC/PC key,then PMC,write down the timer,keep relay,counter and Data details also save all your work program.when you done all this then i'll sent you the lists to set up also give me your parameter 9111 bits No so i can give you correct Option No to set up the Macro B option.

[Dan Fritz]

There'a a special procedure for entering option parameters in the 10 control. You have to enter the parameter in hexadecimal, so take the 8 bits of parameter 9111 that you want to enter (including the "1" for bit #0), and convert it to 2-digit Hex. Then:

Turn off the control
Hold the (-) an the (.) keys
Turn on the control (a 6-choice menu will appear)
Enter "99" then hit INPUT
At the prompt "Axes?" enter the number of axes, then hit INPUT
At the prompt "Option 01" just press INPUT to keep the current value of parameter 9100
At the prompt "Option 02" just press INPUT to keep current value of parameter 9101
(keep pressing INPUT until you get to "Option 12" for parameter 9111)
Enter your new hex value for parameter 9111 and press INPUT
(keep pressing INPUT until all options are entered) Some 10s have 16 options, some have 32

When you get back to that 6-choice menu again, press (I believe) #6 to exit.

The control should then return to normal operation, and you can check to see if option parameter 9111 is set correctly.


NOTE: Its always a good idea to backup ALL the parameters, programs, offsets, etc. before messing around with the option parameters. MACRO B is an option that requires the control to re-map some of the internal memory, so there's a chance that adding an option like this will mess up some of the other memory.

[the professor]

I would like to add, copy any possibly hidden programs o8000 to o8990 and especially any tool change programs in o9000 and above. You may have to change a parameter to see, edit or punch them. Like Dan Fritz said changing this macro B option warns you that all will be gone in memory.
You really don't want to be asking "Does any one have a machine like mine, I lost my tool change programs in o9001, o9002 ,o9003,ect."