Fanuc 6TB g71/g72 canned cycles not canceling U or W after finishing cycle

When I use either the G71 or G72 canned cycles with U and W stock relief the control won't "give me back" either the U or W amount (depending on G71 or G72) when the cycle finishes (G70).
If I use the G71 (linear roughing) cycle the U works just fine but if I have a W100 in the line when the machine returns to the start position the W collects up incrementally. So if I were to run that particular roughing cycle over and over I would collect up an incremental Z of +.010 each time it runs and returns to the start position (4 cycles=.040). I do not run my programs from "G28 HOME" I use a G28 home position in my programming only at the beginning of the program to set the "Start" position closer to the work pc.
G72 (face roughing) is tho opposite, the W works fine but I collect up X+ increments each cycle. I figure it has to be in the parameters somehow because I had this same control on another lathe I worked with and the canned cycles worked just fine with both U and W.

Sorry if my explanation is a bit confusing...I'm a bit confused most of the time anymore.

JohnF
Phoenix

Post your program.
And W100 is not correct. Provide decimal values in mm or inch.

I use 4 place non-decimal values with U and W instead of decimal in any of my incremental canned cycles. In some instances the control will not accept or react to decimal values. W100 (4 place, no leading 0) = W.01(decimal) all inch values. I've been running this particular machine for 15 years and the 6 series (lathes and mills) for almost 25 years. I do what I need to for it to work.

This program will leave +.01 in the Z axis on return to start.

G50 X8. Z5.
T101
G0 X12.5
Z.1
G71 P100 Q101 D1000 U100 W100 F20.
N100 G0 X12.5Z-.7
G1X12.005 F10.
Z-.25 I-500
X10.5
Z.01 I-500
N101U-.1
G70 P100 Q101
G0 X8. Z5. T100
M5
M30

Sorry. I have no experience on this control. But, I am sure somebody would help you.

Quote:

---

Originally Posted by JohnF

When I use either the G71 or G72 canned cycles with U and W stock relief the control won't "give me back" either the U or W amount (depending on G71 or G72) when the cycle finishes (G70).
If I use the G71 (linear roughing) cycle the U works just fine but if I have a W100 in the line when the machine returns to the start position the W collects up incrementally. So if I were to run that particular roughing cycle over and over I would collect up an incremental Z of +.010 each time it runs and returns to the start position (4 cycles=.040). I do not run my programs from "G28 HOME" I use a G28 home position in my programming only at the beginning of the program to set the "Start" position closer to the work pc.
G72 (face roughing) is tho opposite, the W works fine but I collect up X+ increments each cycle. I figure it has to be in the parameters somehow because I had this same control on another lathe I worked with and the canned cycles worked just fine with both U and W.

Sorry if my explanation is a bit confusing...I'm a bit confused most of the time anymore.

JohnF
Phoenix

---

Hi John,

I have the exact same problem on one of the two Mori Seiki SL-7 machines we run, both have Fanuc 6T-B Controls and one works fine while the other increments the X or Z depending on which cycle is used and if I have an offset in either U or W.
We contacted Fanuc but they couldn't find any reason for the increment, I believe it's a error in the Fanuc software, the control with the problem is a slightly older version than the other one which makes me think the bug was fixed in later versions.

Regards,

Quote:

---

Originally Posted by FrankCNC

Hi John,

I have the exact same problem on one of the two Mori Seiki SL-7 machines we run, both have Fanuc 6T-B Controls and one works fine while the other increments the X or Z depending on which cycle is used and if I have an offset in either U or W.
We contacted Fanuc but they couldn't find any reason for the increment, I believe it's a error in the Fanuc software, the control with the problem is a slightly older version than the other one which makes me think the bug was fixed in later versions.

Regards,

---

Makes sense, this is a 1980 machine. I believe that's about when they went to the B version.

Thanks

the program is correct. note only the D can't have a decimal. the U/W should work fine with a decimal (I worked and programmed CNC's including F3/F6 up to 32i's for ~30 years)

you are correct about it being a software bug. you could potentially fix it yourself by updating the software. if you have an EPROM programmer and UV eraser, buy some new blank EPROMs (or buy old ones and erase them), pull the EPROMs from the working machine and program the data to the blanks. Plug'em in, power on and it should fix your issue. Be sure to back-up all parameters first, of course ;-)
and DON'T re-use (i.e. erase and re-program) the old buggy EPROMs. If it doesn't work, simply put the old EPROMs back and live with it.