[mosator]

Hi I generated a g-code for my drilling work but ran to this error in mach3
"R Less Than Z in Cycle in XY Plane"
and i don't have a clue
this is parts of the g-code

G90 G94 G91.1 G40 G49 G17
G21

G0 Z15.00
M3
G4 P4.0
G98 G81 X0.00 Y0.00 R-6.00 Z0.00 F1000.0
X0.67 Y0.53
X0.88 Y1.12
X0.80 Y1.70
X1.41 Y2.16
X1.98 Y2.11
X2.38 Y1.62
X2.16 Y1.04
X2.75 Y1.04
X3.36 Y1.26

NOTE: When i change r to a bigger number than z instead of going down and drill and going up it goes up and moves in down

[mosator]

?

[mosator]

Anyone?

[lucaswalker]

Your position when the drill cycle is called is Z15.0 and the holes goes to Z0.0, if you call a retracion at R-6.00 its makes no sense cause this position is under your start position and even under the bottom of your holes

What is your holes Z top and Z bottom ?

[mosator]

Your position when the drill cycle is called is Z15.0 and the holes goes to Z0.0, if you call a retracion at R-6.00 its makes no sense cause this position is under your start position and even under the bottom of your holes

What is your holes Z top and Z bottom ?

Thank you very much for responding
I changed z to z-15 but still the same error
and if i change numbers to R+6 and Z+15 it's just goes up and moves in down
what should i do to make it right?

[Heavy_Metal]

Hi,

I don't know what G91.1 is doing ??

Try this;

G90 G0 Z15.

G98 G81 X0. Y0. R6. Z0. F----
X--- Y----
X--- Y----

[mosator]

Hi,

I don't know what G91.1 is doing ??

Try this;

G90 G0 Z15.

G98 G81 X0. Y0. R6. Z0. F----
X--- Y----
X--- Y----

Hello
Thank you for responding
I'v done that and it just doesn't move in z axis no more.

[machinehop5]

...R is the reference plane and Z is drill depth. Q is peck distances

N87 T5
N88 S2200 M03
N89 G00 G90 G54 X-146.05 Y-6.35
N90 G43 H5 Z2.54 M08
N91 G83 G98 X-146.05 Y-6.35 Z-15.504 R2.54 Q2.553 F447.04
N92 X-113.594
N93 X-81.139
N101 M09
N102 M05
N103 G53 Z0.
N104 G53 X0. Y0.
N105 M01

[mosator]

my problem is that if z axis is vertical and when negative goes up how can i drill with this g-code? it just doesn't makes sense

[machinehop5]

my problem is that if z axis is vertical and when negative goes up how can i drill with this g-code? it just doesn't makes sense

...you do not have a G Code problem...you have a Z Axis backwards problem

[lucaswalker]

I think you misunderstand how drill cycles works :

there is 3 key z position in the cycle :

1) the Z position when you call the cycle
2) the Z called during the Gxx command of the cycle, which is the depth
3) the R which is the retraction position, the position you will go back before doing a new cycle.

All this can be absolute (G90) or relative (G91) with respect to the initial point (1)

this could be a correct example of your code :

G90 G94 G91.1 G40 G49 G17
G21

G0 Z2.00
M3
G4 P4.0
G98 G81 X0.00 Y0.00 R2.0 Z-5.00 F1000.0
X0.67 Y0.53
X0.88 Y1.12
X0.80 Y1.70
X1.41 Y2.16
X1.98 Y2.11
X2.38 Y1.62
X2.16 Y1.04
X2.75 Y1.04
X3.36 Y1.26

[Superman]

You say that your Zup is negative.... then your programming is $hit
G90 G94 G91.1 G40 G49 G17
G21

G0 Z15.00 ....this is initial level must be higher than R
M3
G4 P4.0
G98 G81 X0.00 Y0.00 R-6.00 Z0.00 F1000.0.... R must be higher than Z
M98 is to return to R, M99 is to return to initial level at the end of each cycle

Get your machine to be correct... ie all Zs above the part are negative or positive.... Not mixed, as you have.

To work out axes, normally, up thru the spindle is Z+, the X is the longest remaining, last is Y. Positive direction is as seen from the operators position. I did say normally,

[mactec54]

Thank you very much for responding
I changed z to z-15 but still the same error
and if i change numbers to R+6 and Z+15 it's just goes up and moves in down
what should i do to make it right?

You can't drill anything with your code like that

G90 G94 G91.1 G40 G49 G17
G21

G0 Z15.00 ( Z axis is above the part by 15mm )
M3
G4 P4.0
G98 G81 X0.00 Y0.00 R-6.00 Z0.00 F1000.0 ( Z0.0=the top of your part so your hole depth is 0.0 deep )

G81G98X0Y0Z-6 R15F1000. ( Now the R value only needs to be enough to clear your work so normally this would be around 3mm to 4 mm )

your Feed rate also is way to high also so start for a lower feed rate


G81G98X0Y0Z-6.0R4.F100.
X0.67 Y0.53
X0.88 Y1.12
X0.80 Y1.70
X1.41 Y2.16
X1.98 Y2.11
X2.38 Y1.62
X2.16 Y1.04
X2.75 Y1.04
X3.36 Y1.26