fanuc 18T

[axis overtravel]

hi all

i run a Daewoo 350M lathe. basic 3 axis machine, X,Z and C with live tooling in 6 of the 12 turret stations, Fanuc 18T controller. the machine was built in 2000.

i want to use polar interpolation, using G12.1/G13.1 to mill a hexagon on the face of a part.

my first question is, am i right in assuming that just because the machine has a programmable C axis, and live tooling, it does not follow that the polar interpolation function is enabled?

my second question is, though i do not have the Fanuc manuals for this machine, reading through a different Fanuc manual, indicates that the polar interpolation axes, linear and rotation, must be set in parameters 5460 and 5461. does anyone have any idea as to what values the parameters need to be set to?

looking at the file of parameters i have downloaded from this machine, 5460 has the value of P1 and 5461 has the value P3

any help would be invaluable

thanks in advance, and a happy new year to you all

[mhed]

have you tried any program with g12? I guess you should use g112 on a 18 control.. g12 works on older versions.

I ve got a macro for hexagon that I could post later if you are interested. Works on fanuc 18/21 , but you must have the macroB option to use it.

[dcoupar]

Here's a PDF with Doosan/Daewoo Polar Coordinate Interpolation instructions, and the section of the F18T-C Parameter Manual dealing with those parameters.

All of the current M type turning centers come with Polar Coordinate Interpolation turned on. I would guess it's turned on in yours, too.

5460 and 5461 sound right. Axis 1= X and axis 3 = C on your machine.

[axis overtravel]

hi mhed

yes, i have tried G12.1/G13.1 and G112/G113. the machine produced a vaguely 6 sided figure, but i guess it could not really be described as a hexagon. if you could post that macro i'll give it a try, thanks

hi dcoupar

many thanks for those pdf's.

i am booked on a training course next week, with the machine's original supplier, so i'm hoping all will be revealed then...

many thanx for your replies...

[mhed]

HEXAGON FACE MILLING ON FANUC 18/21 USING MACRO B.

Example:

Stock dia 100mm.
tool dia 25mm
--------------------------------
Start up c-axis and tool rotation,
etc..

G00 X129 Z-10 (x= stock + tool dia + (2x clearence dist.)
G65 P9020 v80 F800 (v= with of hex, f=feed)

tool returns to same position as in the startup block.
-------------------------------------------------------
Ex 2

G0x129 z0
g66 p9020 v80 f800
z-10
z-20
z-30
z-40
g67
------------------------------------------------------


%
O9020(HEXAGON/M110)
IF[#9LE0]GOTO50
IF[#22LE0]GOTO50
M88 (just for puma, clamping the anti vib. brake)
#29=#9*0.5
#2=0.577
#3=#2*#22*0.5
#5=#5001
#24=#22*0.5
#25=#3*#3
#26=#24*#24
#27=#25+#26
#23=SQRT[#27]
#30=#22
G112
#28=#3-1
G1G41F#9C-#28X#30
X#22C-#3
X0C-#23
X-#22C-#3
X-#22C#3
X0C#23
X#22C#3
C-#3
G1G40X#5C0
G113
M90 ( this is just for puma, unclamp of brake)
G0
M99
N50 #3006=1(value missing)
M30
%

[andys2006]

When I turn my SSO to zero on the OM-VTL I run, the table continues to turn, slowly but still turns, is there a parameter that can be adjusted so that it stops when turned to zero? What parameter is it? thanks- wasnt sure where to put this post