C-AXIS LATHE

[Dtm]

Good morning. I have a problem with the c-axis going the wrong direction. This doesn't matter for most of the parts I have done, however this casting I have to make it does matter. The c-axis is moving the opposite way than it is in verify. Is it a setting in the control def.?

[K2csq7]

There is one in the machine def, double click on the rotary axis and you will see CW or CCW.

Although I am not sure if you will need to make a change in the post for this or not.

[Dtm]

There is one in the machine def, double click on the rotary axis and you will see CW or CCW.

Although I am not sure if you will need to make a change in the post for this or not.

 

Thanks. It still posted the same numbers. I will try to just manually reverse the c values.

[Guest]

If this is a newer post, there is a table in the post that will control it.

 

if this is a purchased post, it may need adjusting by the post builder

[Dtm]

I'm using the Generic Fanuc 4x MT lathe post. I reversed all of the C values and the machine did the same thing. I tried reversing the chain and still the same thing. The machine is trying to take the short route rather than go all the way around. Could someone post this out for me to compare? All of the c-axis toolpaths are good except the last one. I put a file called c-axis on the ftp site in the x5 files folder.

[K2csq7]

%

O0001

(PROGRAM NAME - 28046_J_20)

(DATE=DD-MM-YY - 28-12-11 TIME=HH:MM - 11:12)

(MCX FILE - C:\DOCUMENTS AND SETTINGS\KEITHG\MY DOCUMENTS\`\`\`\`\C-AXIS.MCX-5)

(NC FILE - C:\DOCUMENTS AND SETTINGS\KEITHG\MY DOCUMENTS\MY MCAMX5\LATHE\NC\28046_J_20.NC)

(MATERIAL - FREE MACHINING STEEL)

G20

(TOOL - 5 OFFSET - 5)

( 3/4 FLAT ENDMILL)

( MILL PROFILE AROUND CASTING )

G0 T0505

M23

M8

G0 G54 X5.78 Z.8

C-11.279

G97 S1000 M52

Z.1

G98 G1 Z0. F10.

X5.995

X6.214 C-11.278

X6.437

X6.6085

X6.78 C-11.279

X6.7801 C40. F169.01

X6.78 C79.999

C120.

C160.

C199.998

C239.999

C280.

C293.978

X6.5471 C293.979 F.05

X6.3182 F10.

X6.0934

X5.9367

X5.78

G0 Z.8

M9

G28 U0. W0. H0. M55

T0500

M30

%

 

 

 

 

^^^Hows that look?

[Dtm]

%

O0001(PROGRAM NAME - 28046_J_20)

G20

(TOOL - 5 OFFSET - 5)

( 3/4 FLAT ENDMILL)

( MILL PROFILE AROUND CASTING )

G0 T0505

M200

M8

G0 X5.78 Z.8

C-11.279

G97 S1000 M204

Z.1

G98 G1 Z0. F10.

X5.995

X6.214 C-11.278

X6.437

X6.6085

X6.78 C-11.279

C293.978 F169.01

X6.5471 C293.979 F.05

X6.3182 F10.

X6.0934

X5.9367

X5.78

G0 Z.8

M9

G0 X10. Z10. C0.

M30

%

 

 

Thanks. Looks like a post problem. I broke the chain into 4 quadrants and made 4 toolpaths and it worked out. This is the incorrect program.

[K2csq7]

No post problem.... you did the same thing I did... but dont make it 4 paths. Just break the arc at a few place (i did 7 @ 40 deg) then rechain. Same path just rechain...

[Dtm]

No post problem.... you did the same thing I did... but dont make it 4 paths. Just break the arc at a few place (i did 7 @ 40 deg) then rechain. Same path just rechain...

 

Thanks. Good to know for the future. The jobs is running now so I will leave it be.

[Colin Gilchrist]

There is another option here, but it isn't necessarily the easiest to use. You can use Canned Text to output a direction M code to force the machine to rotate in the direction you want.

 

I modified the Canned Text options in the Control Definition for #21 and #22 to output a direction M Code. (You don't really have to modify the name in the CD, but it helps you when selecting the Canned Text options).

 

Then in the 'Bad' operation, I when into the Chain Manager, and selected "Change at Point". I picked the endpoint at the End of the arc, then in the Change at Point dialog, I enabled the Canned Text option. In the Canned Text Dialog, I selected "M21 (CCW)" + Before.

 

This is how the code came out:

 

%
O0001
(PROGRAM NAME - 28046_J_20)
(DATE=DD-MM-YY - 28-12-11 TIME=HH:MM - 14:37)
(MCX FILE - C:\USERS\CMG\DOCUMENTS\C-AXIS.MCX-5)
(NC FILE - C:\USERS\CMG\DOCUMENTS\MY MCAMX5\LATHE\NC\28046_J_20.NC)
(MATERIAL - FREE MACHINING STEEL)
G20
(TOOL - 5 OFFSET - 5)
( 3/4 FLAT ENDMILL)
( MILL PROFILE AROUND CASTING )
G0 T0505
M23
M8
G0 G54 X-5.78 Z.8
C-11.279
G97 S1000 M52
Z.1
G98 G1 Z0. F10.
X-5.995
X-6.214 C-11.278
X-6.437
X-6.6085
X-6.78 C-11.279
M21
C293.978 F169.01
X-6.5471 C293.979 F.05
X-6.3182 F10.
X-6.0934
X-5.9367
X-5.78
G0 Z.8
M9
G28 U0. W0. H0. M55
T0500
M30
%

 

FYI,

 

The switches in the Machine Definition for the Rotary Axis properties are not hooked up in the Generic Fanuc 4X_MT Lathe Post.

[Dtm]

No post problem.... you did the same thing I did... but dont make it 4 paths. Just break the arc at a few place (i did 7 @ 40 deg) then rechain. Same path just rechain...

 

I just rechained like you said and worked like a charm. This is a strange workaround, but it works.

[K2csq7]

"Shortest direction"