When executing the program my spindle goes down only once to 0.25” then ignores the tree additional
lines and the executes the rest.
I tried adding R0 values on lines with Z values with the same effect.
So I tried rewrite the program:
G84.1G99R+0.6Z-0.25F1000.1Q0.05X0Y0
X0Y0Z-.50
X0Y0Z-.75
X0Y0Z-1.0
G80
G98
M9M5
G0Z2.
Y4.
....the rest of program.....
When executing the program my spindle also goes down only once to 0.25” then ignores the tree
additional lines and then executes the rest.
I made a long shot and rewrote the program again changing the X value only 0.00001”(ten millionths).
This should not make any detectable measurable difference.
To:
G84.1G99R+0.6Z-0.25F1000.1Q0.05X0Y0
X0.00001Y0Z-.50
(went back to X=0)
X0Y0Z-.75
(and then went back to X=0.00001)
X0.00001Y0Z-1.0
G80
G98
M9M5
G0Z2.
Y4.
…....the rest of program.....
To my surprise the program was executed properly making all four pecks.
The thread looks OK.
Then I changed X value only 0.000001 (one millionth).
Program also executed properly.
Big question:
Why my controller does not execute peck cycles while X and Y do not change?
What is proper programing for peck tapping on CNC 88HS.
It works.
In addition I have to use M45 after all next pecks.
So my program looks like this:
….... Code for drilling........
( TAP 1/4- 20 )
M6T2
G0G90S1000.1M5G80M90
G8
G84.2
H2M8Z2.
G84.1G99R+0.6Z-0.25F1000.1Q0.05X0Y0
Z-0.5
M45
Z-0.75
M45
Z-1.0
M45
G80
G98
M9M5
G0Z2.
Y4.
…....the rest of program.....
It also works like this which is more understandable:
….... Code for drilling........
( TAP 1/4- 20 )
M6T2
G0G90S1000.1M5G80M90
G8
G84.2
H2M8Z2.
G84.1G99R+0.6Z-0.25F1000.1Q0.05X0Y0
( Execute the same routine: “M45” but at new Z :“Z-0.5”)
M45Z-0.5
( Execute the same routine: “M45” but at new Z: “Z-0.75”)
M45Z-0.75
( Execute the same routine: “M45” but at new Z: “Z-1.0”)
M45Z-1.0
G80
G98
M9M5
G0Z2.
Y4.
…....the rest of program.....
I guess I never new about code M45 even though it is in my User's Manual.
Thanks again.