G18 help

[AstroReverie]

Fagor 8065 control:

Im programming a radius to run on the X,Z axis while stepping over on the Y-axis. When engaging G18 the Y and Z axis positions change and the machine will give an error if a Z position is entered. Im not running any offsets or cutter compensation. Ive also tried running a Bobcad generated program using the proper post processors and it errors out. Some help with a solution would be much appreciated.

Ive attatched some photos of an example. One showing my position in G17 then the other at the same exact position but with G18 called.
G17 positions are Y-0.1435 Z-0.4254
G18 called shows those positions as Y-5.1373 Z4.8355

Thanks!

 

[GENERALDISARRAY]

1.5 inch long line with a .5r arc in the middle of it. Its just following a line, not a surface.
%
O0
(G18ARC SAMPLE)
(DATE=DD-MM-YY - 31-05-23 TIME=HH:MM - 12:55)
(MCX FILE - T)
(MATERIAL - ALUMINUM INCH - 2024)
(T1|1/4 BALL ENDMILL|H1|D1|TOOL DIA. - .25)
G20
G0 G17 G40 G49 G80 G90
(1/4 BALL ENDMILL|TOOL - 1|DIA. OFF. - 1|LEN. - 1|TOOL DIA. - .25)
T1 M6
B0
G0 G90 G54 X.75 Y0. S4000 M3
G43 H1 Z8.
M8
Z.2
G1 Z0. F15.
X.5 F10.
G18 G2 X0. Z.5 I-.5 K0.
X-.5 Z0. I0. K-.5
G1 X-.75
G0 Z8.
M5
G91 G28 Z0. M9
G28 X0. Y0.
M30
%

 

[AstroReverie]

1.5 inch long line with a .5r arc in the middle of it. Its just following a line, not a surface.
%
O0
(G18ARC SAMPLE)
(DATE=DD-MM-YY - 31-05-23 TIME=HH:MM - 12:55)
(MCX FILE - T)
(MATERIAL - ALUMINUM INCH - 2024)
(T1|1/4 BALL ENDMILL|H1|D1|TOOL DIA. - .25)
G20
G0 G17 G40 G49 G80 G90
(1/4 BALL ENDMILL|TOOL - 1|DIA. OFF. - 1|LEN. - 1|TOOL DIA. - .25)
T1 M6
B0
G0 G90 G54 X.75 Y0. S4000 M3
G43 H1 Z8.
M8
Z.2
G1 Z0. F15.
X.5 F10.
G18 G2 X0. Z.5 I-.5 K0.
X-.5 Z0. I0. K-.5
G1 X-.75
G0 Z8.
M5
G91 G28 Z0. M9
G28 X0. Y0.
M30
%

Tried a similar program and it doesn't work. Here is a shot of a quick cad generated program that wont run on the mill because it errors out due to the machine thinking the Y and Z axis are in a much different position than it actually is.

 

[sinha]

When engaging G18 the Y and Z axis positions change and the machine will give an error if a Z position is entered.

Are you sure?

 

[13engines]

From here it looks like that radius is just that, a radius of some single arc length. You should be able to describe that radius in a single line of code, and not need 5 lines for each pass. Is it not as it appears?

How are you running this without any offsets? Your toolpath lays on the feature surface. You'll need either cutter comp or at least a tool height offset bump of the ball end radius. Running without G43? The nerve! :-)

EDIT IN: Is your machine setup and/or capable of 3 axis simultaneous movement?
What exactly are the errors that appear? Spell them out?

 

[AstroReverie]

From here it looks like that radius is just that, a radius of some single arc length. You should be able to describe that radius in a single line of code, and not need 5 lines for each pass. Is it not as it appears?

How are you running this without any offsets? Your toolpath lays on the feature surface. You'll need either cutter comp or at least a tool height offset bump of the ball end radius. Running without G43? The nerve! :-)

It is just a radius. The way the post processor processes it though - is it puts a small rad on the corners of the starting points of the radius, which is what you're seeing there. The cutter compensation was done in the processing rather than using G41. G43 isn't an existing code on this machines control - it errors out if you apply G43.

I'm still fairly new to this machine and using G-code. I moved over to this machine this last October when we bought it new. Moved over from a Dynapath E422 with, well.. dynapath control which is completely different than Fagor8065 control. I'm currently running the radius on the bottom of this part using a 1/2 Ballnose Endmill. This is how I manually had to write it so that it wouldn't error out the machine using G18 to run just a radius on my X and Z axis while stepping over on my Y axis:

M6 T10
;1/2 BNEM
M3 S8500
G0 G90 X-2.985 Y0.25 Z1
M8
Z0.25
G01 Z0 F150.
Z-0.4254
N1:
G17 G91 Y-0.008 F175.
G90
G18 G03 R10.688 X2.985
G17 G91 Y-0.008
G90
G18 G02 R10.688 X-2.985
N2:
#RPT [N1,N2, 291]
G17 G0 G90 Z1
M9 M5
M98
M30

 

[AstroReverie]

From here it looks like that radius is just that, a radius of some single arc length. You should be able to describe that radius in a single line of code, and not need 5 lines for each pass. Is it not as it appears?

How are you running this without any offsets? Your toolpath lays on the feature surface. You'll need either cutter comp or at least a tool height offset bump of the ball end radius. Running without G43? The nerve! :-)

EDIT IN: Is your machine setup and/or capable of 3 axis simultaneous movement?
What exactly are the errors that appear? Spell them out?

The error it gives is "wrong arc for the programmed radius." Which isn't true.

 

[Vancbiker]

It is just a radius. The way the post processor processes it though - is it puts a small rad on the corners of the starting points of the radius, which is what you're seeing there. The cutter compensation was done in the processing rather than using G41. G43 isn't an existing code on this machines control - it errors out if you apply G43.

I'm still fairly new to this machine and using G-code. I moved over to this machine this last October when we bought it new. Moved over from a Dynapath E422 with, well.. dynapath control which is completely different than Fagor8065 control. I'm currently running the radius on the bottom of this part using a 1/2 Ballnose Endmill. This is how I manually had to write it so that it wouldn't error out the machine using G18 to run just a radius on my X and Z axis while stepping over on my Y axis:

M6 T10
;1/2 BNEM
M3 S8500
G0 G90 X-2.985 Y0.25 Z1
M8
Z0.25
G01 Z0 F150.
Z-0.4254
N1:
G17 G1 G91 Y-0.008 F175.
G90
G18 G03 R10.688 X2.985
G17 G1 G91 Y-0.008
G90
G18 G02 R10.688 X-2.985
N2:
#RPT [N1,N2, 291]
G17 G0 G90 Z1
M9 M5
M98
M30

I don’t know Fagor programming, but seems to me that a G1 as shown in red above should be in your code.

 

[AstroReverie]

I don’t know Fagor programming, but seems to me that a G1 as shown in red above should be in your code.

Just tried it with G01 as well in the line (I did forget to put it in) it didn't change anything though. Ran exactly the same. Good practice to remember to put it in though! Ha.

 

[sinha]

Are you are saying that G01 does not make any difference?

 

[AstroReverie]

View attachment 397514
Are you are saying that G01 does not make any difference?

Yes, G01 didn't change anything. The machine still steps over Y-0.008 with G01 or without G01 in the line. This program you're looking at works. I've milled hundreds of parts with it. I'm trying to figure out why the machine is showing a different position readout than its actually at on the Y and Z axis while G18 is engaged. With it doing that I cannot run Cad processed programs on the G18 or G19 planes because the Cad processed programs interpolate the radius and or angles which makes the machine think the radius or angles are programed wrong which in fact they arent. It also makes watching your position in first op to ensure no crashing impossible because you dont actually know where you are in numbers by watching the readout.

 

[AstroReverie]

@Vancbiker @sinha @13engines @GENERALDISARRAY

I've figured it out. Its tool length compensation (as you said 13engines G43,) except for some reason G43 isn't an active code in the control. I referred to the programming manual and the help menu on the machine and it says to use #TLC[length].. I tried that and the machine gave an error saying "software option is now allowed." Which is strange since it prompts me about it as soon as I start entering it into the program code. I've sort of tricked it by using a fixture offset to compensate for my length on my corresponding axis'. I guess I'll need to dig a little deeper and figure out the proper way to do it for this machine and control.. Still learning as I go. Thanks for all your guys input!

 

[Vancbiker]

One of the drawbacks to not using a “mainstream” control. With so few users it’s hard to get solid assistance.

 

[AstroReverie]

One of the drawbacks to not using a “mainstream” control. With so few users it’s hard to get solid assistance.

Definitely agree. I just found the right code for it. The answer to my problem is #TOOL AX[Z+].

 

[13engines]

The answer to my problem is #TOOL AX[Z+].

Wow... now there's a mouth full.

 

[Vancbiker]

Wow... now there's a mouth full.

Not surprised. It is a Euro control after all.

 

[AstroReverie]

@Vancbiker @13engines

Yeah, I'm not sure why G43 isn't part of the machine control. Pretty basic and useful G-code.