DOOSAN TT1800SY - 18I FANUC - G76 NOT ACTING CORRECTLY

[MMSERV]

I'm running an ID thread on a Doosan TT1800SY which has a Fanuc 18i control. The G76 threading cylce seems to not be working properly.

Here is the code:

G76 P010029 Q50 R40
G76 X-2.400 Z-3.265 P980 Q160 F1.6666

The problem is that the infeed for each pass is only .005 per side. This means that I will have 18 passes to cut this thread. I don't mind the extra time, but the inserts want more of a cut than .005 per side.

It seems that the infeed is actually restricted on the high side by the Q word in the first line of the G76 command. If I change the Q word in the first line to Q100, the result will be an infeed of .010 per side for each pass. This can't be correct, or am I just nuts to think that fanuc should actually vary the infeed depth as advertised.

It seems that the dmin is actually the depth of cut for each pass...

Please help.

Josh

[dcoupar]

I've never seen a thread on a Doosan TT with major diameter of X-2.400... actually never seen X- in a Doosan - only on an old upside down Mori Seiki.

What is the X position prior to the G76 blocks?

[MMSERV]

X-2.0 is the starting X position.

I'm cutting a left handed thread on the ID. I've run this same code on the x positive side of centerline and got the same result. The infeed is exactly the value specified in the first Q variable with the exception of the first, second, second to last and last pass.

Matter of fact here is what the control stated each pass:
2.236
2.249
2.259
2.269
2.279
2.289
2.299
2.309
2.319
2.329
2.339
2.349
2.359
2.369
2.379
2.389
2.392
2.400

(I left of the tenths, they were all .0005 except the second to last and final pass)

Doosan no help, Fanuc no help. Is this the way this canned cycle works? Infeed is the Q? If that is the case why call it 'minimum depth of cut'? I'm at a loss here...

[MMSERV]

Anyone?

[dcoupar]

According to the formula for depth of pass in the 18iT manual, I believe it's working correctly.

The 1st pass is 0.016 deep per Q160 in the 2nd G76 block.
The 2nd pass is decreased to 0.0066 deeper (.016*
The 3rd pass is decreased to 0.0051 deeper
The remaining passes are clamped at 0.005 per Q50 in the 1st G76 block until the next-to-last pass, which is decreased to leave 0.004 per the R40 finish allowance in the 1st G76 block.

One way to achieve your deeper passes would be to "lie" to it and program a larger P and Q in the 2nd G76 block. If you used P1200 and Q350, the passes should be as follows:

2.23
2.259
2.281
2.3
2.3165
2.3315
2.3452
2.358
2.37
2.3814
2.3922
2.392
2.4

[txcncman]

According to the G-code and resulting X positions posted, there is nothing to help with because it is correct. The amount cutting is varying. If you want minimum cut of 0.010, then change Q in first line as indicated. In the first line P word, 00 selects a certain cutting pattern (I do not recall which one and do not feel like looking it up - but you can). I think there are 4 additional cutting patterns (on most machines) that can be selected: 01, 02, 03, 04.

I am still trying to figure out what thread has a 1.6666 inches per revolution lead.

[dcoupar]

[QUOTE=txcncman;1099658]In the first line P word, 00 selects a certain cutting pattern (I do not recall which one and do not feel like looking it up - but you can). I think there are 4 additional cutting patterns (on most machines) that can be selected: 01, 02, 03, 04.
QUOTE]

According to the manual, you have to program the G76 using the F15 (single block) format to make use of the additional infeed types. And it appears there is only P1 (regular) and P2 (staggered) available on the 18.

[MMSERV]

Txcncman,
Good catch, it's .16666 for a 6P Acme. I have resorted to the g92 threading cycle so I could specify exactly how much to take per pass. I guess I just thought the g76 was more robust than it actually is.

[MMSERV]

dcouper,
I like your idea of increasing the P and Q in the second line. I will have to give that a try. Thanks for sharing.

[dcoupar]

dcouper,
I like your idea of increasing the P and Q in the second line. I will have to give that a try. Thanks for sharing.

Another option would be to use G92 which would give you total control over the depth of pass.

[MMSERV]

Ended up using G92 for this one; worked just fine.

Thanks for the input.

[Anders6612]

On the Puma i worked on before, 29 degrees of flank cut was
impossible, only 60 and 55 degrees.