Colchester 2000L Fanuc 0T

The machine has recently lost all its memory, we have got it back up and running with a list of parameters we scrounged from somewhere but various G codes no longer seem to work i.e. G70, G71, G72.

When we use the G71 it returns a "P/S Alarm 065", we're pretty sure the programming syntax we're using is correct.

We think that a parameter needs setting to activate "multi repetitive cycles", anyone got any idea?

I would check your program again just to make sure this is what the alarm in the book says

065 ILLEGAL COMMAND IN G71–G73

1. G00 or G01 is not commanded at the block with the sequence number
which is specified by address P in G71, G72, or G73 command.
2. Address Z(W) or X(U) was commanded in the block with a sequence
number which is specified by address P in G71 or G72, respectively.
Modify the program

We have gone right back to basics and tried the example code in the machine manual for using the G71 cycle, and we still get the alarm message Here is the code:

N10 G21
N20 G95 G00 G40 X400. Z400. T0100 M03
N30 G00 X135. Z150.T0101 M08
N40 G01 X-1.6. F.25
N50 G00 X132. Z152.
N60 G71 U5. R1.
N70 G71 P90 Q150 U1. W.25 F.25
N80 G00 X36.
N90 G01 X50. Z145. F.15
N100 Z120.
N110 X80. Z85.
N120 Z65.
N130 G02 X120. Z45. R20.
N140 G01 X130. Z40.
N150 G00 X400. Z400. T0100
N160 G95 G40 X400. Z400. T0300 M03
N170 G41 G00 X132. Z152. T0303
N180 G70 P90 Q150
N190 G40 G00 X400. Z400. T0300
N200 M30

What kind of machine and model control do you have?

Stevo

(The opinions in this post are my own and not those of machinetoolhelp.com and its management)

Machine is Colchester 2000L Lathe

Controller is a Fanuc 0Ta

If the canned cycles were not activated in the control then you would get an "improper G-code" alarm when trying to run it. It is probably the syntax. It appears that you are using G-code system A.

I am not a whiz with canned cycles especially on a lathe (more of a macro guy). But a quick look at your code, a few things to try.

Change P90 to P80 see what you get. I also think you may need to change your P150 to P140.

Stevo

(The opinions in this post are my own and not those of machinetoolhelp.com and its management)

Thanks Stevo, tried that but still getting the same error code - totally stumped!!!

Ok as I stated before I am not a whiz at canned cycles. Try this code here. I changed P90 to P80 and P150 to P140. I also added the D1. to the G71 line. I am not sure if it is needed but this is your pick size; adjust it to fit your needs. I also removed all the N() addresses at the beginning of the lines. Again I am not sure if it will matter but it is just adding to confusion. The addresses are a waste of space and not needed. They are only needed to specify the start and stop lines of the canned cycle.

G00 X132. Z152.
G71 U5. R1.
G71 P80 Q140 U1. W.25D1. F.25
N80 G00 X36.
G01 X50. Z145. F.15
Z120.
X80. Z85.
Z65.
G02 X120. Z45. R20.
N140 G01 X130. Z40.
G00 X400. Z400. T0100
G95 G40 X400. Z400. T0300 M03

I also want to make sure of the G-code system you are using. What parameter bit is set to 1? 36.1 or 36.5?

If this does not work for you I will PM someone to come chime in that will be able to help.

Stevo

Edit: Just to clarify the alarm code you are getting appears that this is a syntax error so we need to work on the code.

(The opinions in this post are my own and not those of machinetoolhelp.com and its management)

Please check Parameter 900-920
LG

hi,
keep cheack xxx bit must be high of parameter xxx.

If high you just send 900 to 923 parameters detail to here.

naval

LG…these parameters are proprietary to Fanuc and should not be posted publicly. Another thing is this is not Matt’s problem. Options that are not activated on Fanuc controls that involve G-codes would give a different alarm then what he is getting. If the option is not installed it would throw out alarm No. 10 stating improper G-code. The alarm that he is getting relates to a syntax error.

Naval….I edited your post and removed the parameter and bit mentioned. Please refer to the site rules on posting proprietary information publicly.
CNC Professional Forums - FAQ/Rules/Policies: Machinetoolhelp.com-CNC Professional Forums FAQ / Rules & Policies

Thanks,
Stevo

(The opinions in this post are my own and not those of machinetoolhelp.com and its management)

Problem solved!

It was syntax related. A G41 (Tool nose radius compensation) was required immediately after the G71 line. The roughing cycle now works.

A Big Thanks to everyone who has helped!

Matt