How to use g84 in g81

[Dick1951]

Hi

For a lathe Okuma LB15,controll osp 5000 gls,I am using a cyclus in G81;for turning longitude,but I dont now the format g84,to thance the conditions wen i am turning.

How can help me.

[fordav11]

standard longitudinal turning cycle is G85
here's an example.....

G0 X3.15 Z0.2
G85 N31 D0.300 F0.015 U0.03 W0.005
N31 G81
G0 X1.0
G1 Z-10.0 F0.014
X3.0
X3.15 Z-12.0
G80

I was never able to get G84 to work on the piece of dog snot I program/operate but here's an example from the manual.....

G84 is used to change rough turning conditions in bar turning cycles
To change the feed to 0.01 and depth of cut to 0.1 when the cutting reaches X2.0, on the G85 line add this.....

i.e. G85 N31 D0.300 F0.015 U0.03 W0.005 G84 XA=2.0 DA=0.1 FA=0.01

Maybe on single turret LB15/OSP5000 omit the A (X=2.0 D=0.1 F=0.01)?

I ended up just programming the entire part long hand and deleting the cycle completely.
More control and a faster cycle time as well.

[Dick1951]

Hi
Many thanks for the answer,I shall try this next week.
Greetings

[Dick1951]

Hi Fordav11,

Few days ago,I was trying your suggestion,but he did'nt.
The manual 2452 says:N....G85 N....
$ G84 XA=(ZA=) DA= FA=
$ XB=(ZB=) DB= FB=
" N or $"-indicates the commands are continuons.
"XA or XB"-specifies the point of changing.
"DA or DB"-dept of cut after changing.
"FA or FB"-feedrate after changing.

So I wash writing:N0101 G85 N0102 D1.5 U0.4 W0.15(values in mm)
N0102 G81
N0103 G01 Z-20 F0.25
$0104 Z-20 FA=0.25
$0105 Z-45 FB=1
N0106 Z-60
N0109 G80
This is turning a bearing with a hole,and before this I thake a position X20
and z0 in G41.
But when he is turning,he does line N0103 with $0104 and $0105 separed,verywell,but only with F0.25 and than he goes to Z-60 also in F0.25.
Thats the qwestion,I don't no.

I'm sorry for the bad Englis.
In Holland we says;I want to learn reading and writing with the machine and
that's wat I want.

Many greetings.

[fordav11]

the result is unexpected because the machine does not understand those commands in those places.

don't put $ on normal program lines.
it means 'add those lines together'
so....
G01 Z-10.0 F0.25
$Z-20.0 F.3

actually means....
G01 Z-10.0 F0.25 Z-20.0 F.3

the later Z and F cancels out the earlier one. on some controls the first Z and F would be read and the later one ignored.

you can't control the cycle depth of cut and feedrate by adding Z values. According to the manual the G84 has to be on the same line as G85