Need Help!- Need help with G75 code on Fanuc 10

[bobancurug]

Hello!

I have a problem with the code G75 on the machine Takisawa TC-3 with the Fanuc 10 system.
The program is already used on the machine Takisawa TC-3 with system
Fanuc 0 and worked without any problems.
When I switched to another machine with the Fanuc 10 system , G75 does not work.
This is part of the program with the G75 where the machine stopped without an alarm, just a stop.

M1
G50X162.36Z247.98S1500
G0G99G96S110T0707M16
X85.Z2.M3
Z-55.8M8
G75R100
G75X70.P300F0.07
G0Z-52.2
G75R200
G75X70.Z-17.65P500Q3612R39F0.11
G0Z-17.65
G1X70.5F0.3
G75R100
G75X55.5P300F0.07
G0Z-21.35
G75X55.5Z-52.2P500Q3612R39F0.11
G0X83.
Z-55.8
G1X70.5F0.3
G75R150
G75X54.5P400F0.12
G0X100.
Z10.
X162.36Z247.98T0000
M1


Is it something that I need to change in the program or the problem may be in the parameters?

Thanks in advance for your responses!

[angelw]

Originally Posted by bobancurug Hello! I have a problem with the code G75 on the machine Takisawa TC-3 with the Fanuc 10 system. The program is already used on the machine Takisawa TC-3 with system Fanuc 0 and worked without any problems. When I switched to another machine with the Fanuc 10 system , G75 does not work. This is part of the program with the G75 where the machine stopped without an alarm, just a stop. M1 G50X162.36Z247.98S1500 G0G99G96S110T0707M16 X85.Z2.M3 Z-55.8M8 G75R100 G75X70.P300F0.07 G0Z-52.2 G75R200 G75X70.Z-17.65P500Q3612R39F0.11 G0Z-17.65 G1X70.5F0.3 G75R100 G75X55.5P300F0.07 G0Z-21.35 G75X55.5Z-52.2P500Q3612R39F0.11 G0X83. Z-55.8 G1X70.5F0.3 G75R150 G75X54.5P400F0.12 G0X100. Z10. X162.36Z247.98T0000 M1 Is it something that I need to change in the program or the problem may be in the parameters? Thanks in advance for your responses!

The format for the O series control uses two lines for the G75 cycle, whereas the 10 series control only uses one block.

The R value in the first line of the O series format sets the Return amount between pecks and is a modal value. This value can also be set in parameter #722 in the O series and remains until changed by specifying another value with G75 R in the program. Accordingly, if you wanted the two machines to have a similar one line format, and you're happy to have a constant retract amount across all G75 applications used with the O series machine, the value can be set in the parameter and the first G75 line in the cycle omitted. However, the series O and 10 control use a different syntax in the main G75 block. Therfore, the programs aren't transportable between the two controls.

The syntax for the G75 cycle for the 10 series machine is as follows:

G75 X(U).... Z(W).... I.... K.... F.... D.... Where:
X = Finish point in X
Z = Finish point in Z
U = Incremental value of X
W = Incremental value of Z
I = Step across movement in Z direction
K = Depth of cut in the X direction
F = Feed rate
D = Relief amount for the tool at the end of the cut in Z.

In the above format, Z,I and D are used if the cycle is to be used to machine a groove wider than the width of the grooving tool, or for a series of holes where the pitch of the holes will be described by I and the last hole coordinate by Z.
1. When used for any drilling operation, parameter D is omitted.
2. When used to drill a single hole Z,I and D are omitted. When omitted, the D parameter is assumes to have a value of zero, and Z and I are ignored in software.

The Return amount set by R in the first G75 line of the O series control format, is set in parameter #6217 of the 10 series control. Unlike the O series, this is the only way the Return amount can be set on a 10 series machine.

Regards,

Bill

[bobancurug]

Thanks Bill for this excellent explanation, tomorrow I'll try to rewrite the program, and also to try that with changing parameters
Thanks again,
Boban

[sinha_nsit]

R in the first block should be in mm/inch, not in micron/thou.

[ESP666]

Can anyone explain what the Q & P values in this line actually mean?

G75X70.Z-17.65P500Q3612R39F0.11

The G75 lines that Im looking at have the format:

G75 X Z P Q F

Cheers for your help!

[angelw]

Originally Posted by ESP666 Can anyone explain what the Q & P values in this line actually mean? G75X70.Z-17.65P500Q3612R39F0.11 The G75 lines that Im looking at have the format: G75 X Z P Q F Cheers for your help!

G75 canned cycle can be used for grooving or drilling in the X axis. The P and Q have the following meanings:

1, P = the peck amount before retracting to chip break.
2. Q = the side steps along the Z axis in a grooving operation, or it could be used as the pitch between holes in the Z axis if being used in a drilling operation. Note: If used in a drilling operation, R must be assigned zero.

Originally Posted by sinha_nsit R in the first block should be in mm/inch, not in micron/thou.

sinha The R in the first block is saved in parameter #722 and is model, ie. the value stays the same until a different value is specified in a G75 block, or changed via MDI. Its stored in units of 0.001mm or 0.0001inches, depending on the configuration of the machine; the range is 0 to 99999999. Unless the control is configured to use Calculator style decimal input (selectable via parameter) the R value in the first G75 block can in fact be specified either with or without a period. If no period is used, the value is considered in terms of the number of least input units.

Whilst there are some arguments that must be specified without a period, all dimensional addresses such as X(U), Z(W), I, J, K, R etc can be specified without a period provided they are padded with the correct number of "0" so that a true representation of the intended value is preserved


Regards,

Bill

[sinha_nsit]

With calculator-type setting, R should be in mm/inch.
Is it correct now?

[ESP666]

Thanks Bill!