threads

[dgchumley]

I'm having a problem with a G76 on an 18-T controller on a Hardinge super precision lathe. My threads are coming out ok but the first pass is very deep.
The format goes something like this....

G76 P---- Q---- R----
G76 X--- Z--- Q---- F----

Please tell me exactly what each of the parameters defines so I can figure out what the problem is.
Thanks alot.

[tobyaxis]

Originally Posted by dgchumley I'm having a problem with a G76 on an 18-T controller on a Hardinge super precision lathe. My threads are coming out ok but the first pass is very deep. The format goes something like this.... G76 P---- Q---- R---- G76 X--- Z--- Q---- F---- Please tell me exactly what each of the parameters defines so I can figure out what the problem is. Thanks alot.

I use this format years ago but can't remember. This is the only fomat I've used for the past few years (see picture at bottom).

If G76 isn't working for you try G92. It will allow you to taylor each cut right down to how many spring passes you want.

Format is as follows:

G40G0X.25Z.05
X.12
G92X.043Z-.05F.01041
X.041
X.039
X.037
X.035
X.034
X.033
X.0325
X.032
X.032
G40G97G0Z.1
G28U0W0T0
M1

[adamant]

G76 P---- Q---- R----
G76 X--- Z--- Q---- F----

If your first cut is deep your starting point could be small. I use .015 from the material for OD or ID.

Mess with your Q's for first pass depth. .................The second Q is for first pass.

You can cut threads so fast that I often just went with Q5 on both numbers. This cuts .001 per pass.

[adamant]

Originally Posted by adamant G76 P---- Q---- R---- G76 X--- Z--- Q---- F---- .

P=02 number of finish passes
00 not sure what this one is........00 is fine
60 Degree of tool point normally 60

top Q= mininum cutting depth

R= finnsih allowence.......small number is good R5

Second Q is the amount of fist pass.

X= Major or minor depending on ID or OD
Z=Leangth

F=feed rate 1/number of threads per inch

[jackson]

This is how i set mine up it does not appear that you have a P in the second line "you may not have to have one but i always use it, its the highth of your thread the Q in the second line controls you first cut depth Q in first line is the amount per pass

N9000
(1/2-20 OD THRD)
G0G55T202
G97S400M3
G0X.55Z.1M8
G76P020060Q70
G76X.4402Z-2.14R-.0015P0620Q100F.05
G0X6.0Z8.M9
M1
M30

[jackson]

here is the format

[Paul in OK]

Old topic, but I would like to know where this attachment came from. Very helpful. Is there something similar to show other G code info in the same manner?
Paul in OKC

[g-codeguy]

Originally Posted by dgchumley I'm having a problem with a G76 on an 18-T controller on a Hardinge super precision lathe. My threads are coming out ok but the first pass is very deep. The format goes something like this.... G76 P---- Q---- R---- G76 X--- Z--- Q---- F---- Please tell me exactly what each of the parameters defines so I can figure out what the problem is. Thanks alot.

You are missing the "P" in the second block. As someone else already stated, the "Q" in the second block is the DOC for the first pass. P in the second block is the thread height (per side).