Hello,
 Trying to use cutter comp in KmotionCNC v4.33. I keep getting an error window. Here is a snippet of code and note where it is faulting. I ran a slightly altered version in Mach4 with no issues. Only reason i altered to what is below was to try and get comp to work in KMotionCNC.
Anyhelp much appreciated,
Thanks,
Troy

(1001)
(T1  D=0.194 CR=0. - ZMIN=-0.535 - FLAT END MILL)
G90 G94  G40 G49 G17
G20
G40

(2D CONTOUR3)
G53G0Z0
G53G0X0Y0
T1 M6
S2500 M3
G54
G0 X-0.5167 Y0.782

G43 Z0.1 H1
G41 D1 <........(Here is where i get the gouging error window)
G1 Z0.0394 F40.
Z-0.125 F12.5

G01 X-0.5784 Y0.6929 F50.
G3 X-0.4146 Y0.625 I0.1638 J0.1638
G1 X0.4146
G3 X0.5784 Y0.6929 I0. J0.2317
G1 G40 X0.5167 Y0.782
G0 Z0.1

(2D CONTOUR3)
G55

G0 X-0.5167 Y0.782
G1 Z0.1 F40.
Z0.0394

................

Hi Troy,

I'm not sure what you are trying to do.  Should that be an inside contour?

I think Mach3/Mach4 are pretty forgiving about allowing gouging the specified path where KMotionCNC is not.  I suppose KMotionCNC could be more relaxed but in certain cases the path becomes undefined and bizarre things can result.

The first Move after turning on cutter compensation should be an "Entry Move" to engage the xy cutter offset.  Your first move seems to be in z.  Actually I get the error on the line after you marked with an arrow.

You might look at this example: 

http://www.dynomotion.com/wiki/index.php?title=Internal/concave_Path_Tool_Radius_Compensation_Example_G41/G42

Regards
TK

 

Hello,
 Trying to use cutter comp in KmotionCNC v4.33. I keep getting an error window. Here is a snippet of code and note where it is faulting. I ran a slightly altered version in Mach4 with no issues. Only reason i altered to what is below was to try and get comp to work in KMotionCNC.
Anyhelp much appreciated,
Thanks,
Troy

(1001)
(T1  D=0.194 CR=0. - ZMIN=-0.535 - FLAT END MILL)
G90 G94  G40 G49 G17
G20
G40

(2D CONTOUR3)
G53G0Z0
G53G0X0Y0
T1 M6
S2500 M3
G54
G0 X-0.5167 Y0.782

G43 Z0.1 H1
G41 D1 <........(Here is where i get the gouging error window)
G1 Z0.0394 F40.
Z-0.125 F12.5

G01 X-0.5784 Y0.6929 F50.
G3 X-0.4146 Y0.625 I0.1638 J0.1638
G1 X0.4146
G3 X0.5784 Y0.6929 I0. J0.2317
G1 G40 X0.5167 Y0.782
G0 Z0.1

(2D CONTOUR3)
G55

G0 X-0.5167 Y0.782
G1 Z0.1 F40.
Z0.0394

................

Hi Tom,
 The actual move is a X axis cut on left side(G41) with a radius lead in and lead out. I usually have my cutter comp feed move with D word and G4? all on same line, but i was getting the gouging error, so i tried to copy an example in KMCNC. What i posted is where i stopped :) Could not figure out why KMCNC was not working with my comp move line.
Mach4 has "tightened" up its code to be more industry Fanuc standard.

Here is the Gcode with only the one feed line move using a Generic FANUC post processor.Iam using Fusion360.
What would be the reason that KMCNC sees the comp move as gouging with the below Gcode?
Thanks,
Troy

%
O1001
(T1 D=0.194 CR=0. - ZMIN=-0.125 - FLAT END MILL)
N10 G90 G94 G17 G49 G40 G80
N15 G20
N20 G28 G91 Z0.
N25 G90

(2D CONTOUR3)
N30 T1 M06
N35 S2500 M03
N40 G54
N45 M08
N55 G00 X-0.5167 Y0.782
N60 G43 Z0.1 H01
N65 G01 Z0.0394 F50.
N70 Z-0.125 F12.5
N80 G41 X-0.5784 Y0.6929 D01 F50.
N85 G03 X-0.4146 Y0.625 I0.1638 J0.1638
N90 G01 X0.4146
N95 G03 X0.5784 Y0.6929 J0.2317
N105 G01 G40 X0.5167 Y0.782
N110 G00 Z0.1

N120 M09
N125 G28 G91 Z0.
N130 G49
N135 G28 X0. Y0.
N140 M30
%

Hi Troy,

Here is the contour path you have programmed showing the first entry move.

At the end of the Entry move the Nist Interpreter positions the tool as if it were following the contour of the Entry Move. 



But then in your case  to follow the Contour without gouging is impossible.

Actually I think I have the tool diameter scale way off but the result is basically the same.

I think the solution might require reducing the length of the Entry Move to stop the gouging.  Then add an arc in the contour slightly larger than the tool radius to merge into the original contour.

Do you know what the Fanuc or Mach4 actually do in that case?

Regards
TK

 

Hi Tom,
 The actual move is a X axis cut on left side(G41) with a radius lead in and lead out. I usually have my cutter comp feed move with D word and G4? all on same line, but i was getting the gouging error, so i tried to copy an example in KMCNC. What i posted is where i stopped :) Could not figure out why KMCNC was not working with my comp move line.
Mach4 has "tightened" up its code to be more industry Fanuc standard.

Here is the Gcode with only the one feed line move using a Generic FANUC post processor.Iam using Fusion360.
What would be the reason that KMCNC sees the comp move as gouging with the below Gcode?
Thanks,
Troy

%
O1001
(T1 D=0.194 CR=0. - ZMIN=-0.125 - FLAT END MILL)
N10 G90 G94 G17 G49 G40 G80
N15 G20
N20 G28 G91 Z0.
N25 G90

(2D CONTOUR3)
N30 T1 M06
N35 S2500 M03
N40 G54
N45 M08
N55 G00 X-0.5167 Y0.782
N60 G43 Z0.1 H01
N65 G01 Z0.0394 F50.
N70 Z-0.125 F12.5
N80 G41 X-0.5784 Y0.6929 D01 F50.
N85 G03 X-0.4146 Y0.625 I0.1638 J0.1638
N90 G01 X0.4146
N95 G03 X0.5784 Y0.6929 J0.2317
N105 G01 G40 X0.5167 Y0.782
N110 G00 Z0.1

N120 M09
N125 G28 G91 Z0.
N130 G49
N135 G28 X0. Y0.
N140 M30
%

Attachments :

250leadin-14005.jpg

I will have to look closer at what happens, as the lead in is far enough away from part that there is no issue that is noticeable when comp is turned on.  I did adjust my lead in to .250 to get KMCNC to accept it but the toolpath looks like that comp is just barely turned on and off. My tool diameter is .194".

I was misunderstanding the gouging error window. Didn't realize that it just needed more lead in for comp.(Duh :)
 Will have to check tomorrow at machine, but i have another part of program that needs to be a much tighter comp move with same tool diameter.
Thanks again,
Troy

Attachments :

Co-Bore CC-14010.jpg

Hi Tom,
I checked how machine runs in Mach4 and i see no issues or gouging with my first gcode.

Below is the 2nd part of Gcode that has a much tighter comp move. This Gcode is doing a Counter Bore spiral down. Also, the attached picture "Co-Bore CC" is Mach4 toolpath screen of the below gcode with cutter comp of an .194" endmill.

When i run this Gcode in KMCNC i get a "Concave corner with cutter radius comp" window, even when i set tool diameter to .001.

Anyway to work around this?
Troy


%
O01001
(T1 D=0.194 CR=0. - ZMIN=-0.2 - flat end mill)
G90 G94 G17
G20
G53 G0 Z0.

(Bore2)
T1 M6
S2500 M3
G56
M8
G0 X0.563 Y0.
G43 Z0.18 H1
G1 Z0.1 F50.
G41 X0.5285 Y0.122 D1
G3 X0.4065 Y0. I0. J-0.122
X0.4071 Y0.0136 Z-0.0479 I0.1565 J0.
X0.7194 Y-0.0068 Z-0.124 I0.1559 J-0.0136
X0.4065 Y0. Z-0.2 I-0.1564 J0.0068
X0.7195 I0.1565 J0.
X0.4065 I-0.1565 J0.
X0.5285 Y-0.122 I0.122 J0.
G1 G40 X0.563 Y0.
G0 Z0.18

M5
M9
G53 G0 Z0.
G53 X0. Y0.
M30

%

Hi Troy,

Here is a new Fanuc style Radius Compensation Entry mode Style that seems to work for your code.

Here is a patch for Version 4.34e to add that as an option

http://dynomotion.com/Software/Patch/AddFanucStyleCompEntryMove_V434e/GCodeInterpreter.dll

Copy it to the C:\KMotion434e\KMotion\Release directory.

See the description of how it works and how to turn on that style here:

http://www.dynomotion.com/wiki/index.php?title=Internal/concave_Path_Tool_Radius_Compensation_Example_G41/G42

Please let us know if you find any issues.

Regards

TK

 

Hi Tom,
I checked how machine runs in Mach4 and i see no issues or gouging with my first gcode.

Below is the 2nd part of Gcode that has a much tighter comp move. This Gcode is doing a Counter Bore spiral down. Also, the attached picture "Co-Bore CC" is Mach4 toolpath screen of the below gcode with cutter comp of an .194" endmill.

When i run this Gcode in KMCNC i get a "Concave corner with cutter radius comp" window, even when i set tool diameter to .001.

Anyway to work around this?
Troy


%
O01001
(T1 D=0.194 CR=0. - ZMIN=-0.2 - flat end mill)
G90 G94 G17
G20
G53 G0 Z0.

(Bore2)
T1 M6
S2500 M3
G56
M8
G0 X0.563 Y0.
G43 Z0.18 H1
G1 Z0.1 F50.
G41 X0.5285 Y0.122 D1
G3 X0.4065 Y0. I0. J-0.122
X0.4071 Y0.0136 Z-0.0479 I0.1565 J0.
X0.7194 Y-0.0068 Z-0.124 I0.1559 J-0.0136
X0.4065 Y0. Z-0.2 I-0.1564 J0.0068
X0.7195 I0.1565 J0.
X0.4065 I-0.1565 J0.
X0.5285 Y-0.122 I0.122 J0.
G1 G40 X0.563 Y0.
G0 Z0.18

M5
M9
G53 G0 Z0.
G53 X0. Y0.
M30

%

Hi Tom,
 Awesome! work. Will give it a go at shop tomorrow and let you know.
Thanks again Tom.
Troy

Hi Tom,
 I copied dll to directory but when i try to launch KMCNC i get a window stating "KMotion CNC MFC Application has stopped working" with options of Check online for a solution and close program, Close Program and Debug the problem.

Did i mis a update to this version of KMCNC?

Thanks,
Troy

Hi Troy,

Oops sorry, this changed also:

http://dynomotion.com/Software/Patch/AddFanucStyleCompEntryMove_V434e/KMotionCNC.exe

Regards

TK

 

Hi Tom,
 Awesome! work. Will give it a go at shop tomorrow and let you know.
Thanks again Tom.
Troy

Hi Tom,
 Tried out new version 4.34e with new Fanuc Comp code on mill, it works great:) Nice and smooth. Is also neat to watch code work in reverse when using the pause reverse button in KMCNC.

Thanks again Tom for your hard work and support.

Troy

Thanks for adding the fanuc style comp option Tom, Will this be included going forward with future release versions, or will a patch be required with future upgrades?

Yes it will be included in the next Test Release.  Note it must be enabled in the Settings File.

Regards

TK

 

Thanks for adding the fanuc style comp option Tom, Will this be included going forward with future release versions, or will a patch be required with future upgrades?