HELP! miyano newbie g74 code error

[ivan13]

trying to program drill peck cycle. i'v only been running this type of machine for two weeks. this is what i have programed. G74 Z-1.0 K-.1 R1 F.003. works on a mori seiki. why not this machine?

[Stevo]

We need more information than that in order to help.

What model control is on your machine?? What happens when you try to run that code? Does the machine alarm out? If so what alarm numbers are you getting?

Stevo

[ivan13]

it's a miyano bnc 34c with a fanuc o.t. control. an older model i belive (MID 90'S). it puts up alarm 65 i belive.

[Stevo]

Here is your alarm description per the Ot manual along with the remedies. It appears that you have a syntax error. Use the 2 suggestions below or post your code here so we can have a look at it.

065 ILLEGAL COMMAND IN G71--G73

1.G00 or G01 is not commanded at the block with the sequence
number which is specified by address P in G71, G72, or G73 command.

2. Address Z(W) or X(U) was commanded in the block with a sequence
number which is specified by address P in G71 or G72, respectively.

Modify the program.

Stevo

[ivan13]

sorry about that. it's a 062 alarm that pops up. i'm use to programing hardinge conquest and mori seiki (with yaznac controls). funny this miyano is like a combination of both, or so it seems.

[Stevo]

No worries.

Attached is the alarm description and cause codes.

It appears that the error is in the code.

Stevo

[angelw]

Originally Posted by ivan13

trying to program drill peck cycle. i'v only been running this type of machine for two weeks. this is what i have programed. G74 Z-1.0 K-.1 R1 F.003. works on a mori seiki. why not this machine?

Ivan13,
The error is in the syntax of your code.

1.The R address in your example is technically legal, but would have resulted in the drill stepping sideways (X axis) at the bottom of the drilled hole. Accordingly, its lucky the control came up with an error, as the alternative may have ended in tears, depending on whether the R1 without a period was intentional. The Fanuc control would have interpreted this as R0.0001" unless the control was configured in Pocket Calculator Mode.

2. K is not a valid argument in this cycle, and I suspect that this is what raised the alarm.

G74 is a Face Grooving, or Peck Drilling cycle, depending on the omission or value of certain arguments. The 0 Series control uses what is now referred to an Standard Series 16 format, wherein the cycle is a two block arrangement. On later controls, Series 15 format can be selected via parameters.

Following is the complete format including the arguments required for machining a Face Groove

G74 R...
G74 X(U)... Z(W)... P... Q... R... F...

Where:
R in the first G74 block = Return amount
This designation is modal and is not changed until another value is designated. This first block can be omitted and the value specified by the parameter #5139. This parameter is changed by the program command.
X = Finish absolute component of face groove
U = Incremental amount in X from Start to Finish diameters of face groove
Z = Absolute depth component of face groove, or drilled hole
W = Increment amount from Start to Finish in Z
P = Movement amount in X direction (without sign), for face groove
Q = Peck depth of cut in Z direction (without sign), for face groove, or drilled hole
R in second G74 block = Relief amount of the tool at the cutting bottom. The sign of R is always plus. However, if address X(U) and P are omitted, the relief direction can be specified by the desired sign.
F = Feed rate

Following is an example to Peck Drill a hole 50mm deep, 5mm pecks, feed rate of 0.150mm/rev, and a Relief amount of 0.25mm specified via the program.

G74 R0.250
G74 Z-50.000 Q5.000 F0.150

Regards,

Bill