G76 Thread problem on Mitubishi 700 control

[pmcguc618]

I get error P204 after the first line below:
G76P010160
G76x.4782z-.9P0307Q0140F.05

any ideas?

[camsys]

I'm guessing you're trying to thread on a lathe.

You might try the second 2 digits in your first P command to be 00, and
add your Q and R to the first line as well.

Check where your start is in X and make sure the X is advanced in the correct direction.

To amke a 1/2 x 13 thread you might do it this way as an example
g97 g95
s500m3
g0g54x.6 z.1
x.5
g76 p030060 q.03 r.02
g76 x .421 z-1.0 r0. p.0395 q.1 f.0769
g0 x1.0

[camsys]

I hit post before finishing the response below.

if you still get an error, you can check parameter #1265.1 and if it is
set to 1, then the G76 would be done in one line:

G76 x z i k d f a q

where the values you provide here would be
x = finish location
z= finish location
i = radius at thread section (probably 0 for you)
k = thread height
d = first pass cut amount
f feedrate
a = thread angle
q = start angle of thread

number of finish passes parameter 8058
finish allowance parameter 8057

[cogsman1]

The "P" and "Q" need a decimal value on that control, as camsys has shown.

[cogsman1]

On the SECOND "G76" line that is. And CAPITAL letters.