FANUC 0i-TC G76 canned cycle.

chip4761 said:

Here's the dilemma. First off, I was not operating the machine when this problem popped up, so I'm sort of flying blind, and I apologize in advance for any information I've overlooked.

We have a 0i-TC on a lathe that was running a G76 threading cycle just fine yesterday on an external thread. At some point, this was copied and slightly altered to do internal threading (this control doesn't have a command to specify internal/external.) Somehow during this process something was changed that shouldn't have been. The question is: What? Neither the original OR copy will run appropriately. It just runs 2 passes at the finish depth (it's set to 2 passes at finish.)

It will run a G71 roughing cycle just fine. Why not the G76? Is there something that could have been altered in the program syntax that I'm just not seeing? Also, is there any way that a parameter could have changed without directly altering it within the parameter settings? That seems exceptionally unlikely to me. Any help would be GREATLY appreciated. Thanks!

Click to expand...

angelw said:

If parameter 0001.1 is set to 1, Series 15 format applies, otherwise Series 16 Standard format applies.

Series 15 format = Single line G76
Series 16 format = Two line G76

I'm assuming that your control is set for Series 16 (default).

Post the code for both your External and Internal thread, including the last X coordinate line prior to calling the treading cycle.

There is no specific command to designate either External or Internal threading. The control determines this by comparing the start X coordinate with the X(U) specified in the second G76 block. For an external thread the X start coordinate must be at least the Minor diameter specified by X in the second G76 block, plus 2P of the same block (thread X + P x 2). The opposite is the case for an Internal thread where the Major diameter is specified by X and P x 2 is subtracted to determine the maximum diameter the tool can start from in X.

Theoretically, it does not matter how far away in X from the thread the tool starts from. Of course, the obvious limiters for an Internal thread is the diameter of the bore, the diameter of the thread cutting bar used, and how far past center line of the machine is the X over-travel.

Following is how the control deals with the X, P and Q of the second G76 block:

1. Whether the thread is Internal or External is determined by the comparison of the X start and the X specified in G76 block. Obviously, the X start coordinate needs to be a larger diameter than the Major diameter of an External thread, and smaller than the Minor diameter of an Internal thread.

2. External example follows:
i. In software, to determine the Major diameter of the thread, the control adds P x 2 (thread height x 2) to the minor diameter specified by X.
ii. The control then subtracts Q x 2 (depth of first threading pass x 2) to calculate an X coordinate for the first threading pass.

The following parameters are changed by the threading cycle itself, and remain model, even after cycling the power On/Off, until changed by the G76 cycle, or via MDI

G76P (m) (r) (a) Q (Δd min) R(d);
G76X (u) _ Z(W) _ R(i) P(k) Q(Δd) F(L)

m = parameter 5142

r = parameter 5130

a = parameter 5143

Δdmin = parameter 5140

d = parameter 5141

If these arguments are omitted, the values stored in parameters apply


Regards,

Bill

Click to expand...

Radian51 said:

Do you have extensive knowledge of Oi TC?


Sent from my iPhone using Tapatalk

Click to expand...