Okuma Lb3000ex 2 IGF C-axis Programming
Hi guys. Im having some trouble getting my machine to do what I want. Im sure its simple but I cant figure it out so I seek some help.
OSP-300l Control
So Im trying to mill in a water jacket using my c-axis with a double lead. I get shape underdetermined when I try and do it.
If anyone would be able to help me Id greatly appreciate it. Honestly prob easiest via phone or text so I can take pictures to explain everything and let you get a vision of what Im trying to do.
Please PM me if your able to help and we can share contact info.
Re: Okuma Lb3000ex 2 IGF C-axis Programming
hy mike :) there are a few code types when using c axis : [ G01 or G101 or G102 or G103 ] + [ X or C or XC ] + [ nothing or Z ], and some others :)
igf is not able to generate all of them
i need to know what kind of toolpath you need; it may be able to generate it using igf, but, if it's simple, it may be faster to write the g-code
kindly :)
ps : maybe share a photo with your actual shape in igf ? or coordinates ...
3 Attachment(s)
Re: Okuma Lb3000ex 2 IGF C-axis Programming
here is the print of what im trying to do.
All I want is my c to rotate at the pitch. flip it 180 and repeat. Just not sure how to make it do it.
1 Attachment(s)
Re: Okuma Lb3000ex 2 IGF C-axis Programming
hy mike :) if you would use an endmill with dia 0.378, then it would be required to cut a helix with a number of loops = (3.8898-0.5512)/0.5315=6.28146...= 2pi
let's round that up, at 7 : this means a clearance of 7-2pi; pls be aware that this clearance is relative to the right side of dimension 3.8898, and this is not your part face ... thus, if you have Z0 on the right, then, before cutting 7 loops, you should shift your Z0
Code:
V1 = rpm
V2 = feed_in_g95
V3 = target_diameter
V4 = turret post
( * )
G00 X_up Z_rigth
T+V4*101
M110
SB=V1 M13 ( M08 )
VZSHZ = - [ 3.9370 - 3.8898 ] + [ 7 - 2 * VPAI ]
G00 X=V3 Z0 C0 ( M15 or M16 )
CALL OSUB Q=7*2
X_above_part G90 F
M12
M109
G00 X_up Z_rigth T+V4*100 VZSHZ = 0
OSUB
G01 Z-0.5315/2 C180 G91 G95 F = SQRT ( ( ( 360 * 0.5315 / 2 ) ^ 2 + ( 500 * 180 ) ^ 2 ) / ( ( 360 * 0.5315 / 2 ) ^ 2 + ( VSIOX * 180 * VPAI ) ^ 2 ) ) * V2
RTS
* at least for this operation, g-code can be written faster than messing with the igf
if your tool dia < 0.378, then is needed to compute each pass ... or, it would be possible to rough towards same Z end, and finish like showen in attached image
what kind of tool do you use? perhaps a custom tool is affordable ...
Quote:
All I want is my c to rotate at the pitch. flip it 180 and repeat.
c & z axis should work syncronuous
by the way, is possible to rough that by using a threading insert, but, after that, is required to "merge" M19 and C origins
kindly :)
Re: Okuma Lb3000ex 2 IGF C-axis Programming
thank you sir! I will give this a try. I do have a custom ground tool to do it with. I appreciate your time.
Re: Okuma Lb3000ex 2 IGF C-axis Programming
ok :) i have edited the code, so instead of cutting 14*180degrees, it now cuts 7*360degrees; this should deliver a smoother movement
i don't know exactly the dimensions of your part, but i suggest you rough with a tool dia < custom tool dia, then pre-finish and finish with your custom tool
something like this :
... cut at X_start - X_depth_rough * 0, with tool_1
... cut at X_start - X_depth_rough * 1, with tool_1
... cut at X_start - X_depth_rough * 2, with tool_1
... etc
... cut at X_start - X_depth_rough * n, with tool_1
... cut at X_end + X_depth_finish * 2, with custom tool
... cut at X_end + X_depth_finish * 1, with custom tool
... cut at X_end + X_depth_finish * 0, with custom tool
* thus just edit V3 inside that program
this should put less stress on the custom tool, thus keeping it's wear to a minimum necessary
tool_1_dia should be < custom_tool_dia ... also, tool_1 may be a bit blunted, it does not matter, as long as it leaves enough material, so your final tool to deliver a smooth surface
at the end, would be ok to run a chamfer tool, in order to debur your edges ... this requires a code that cuts on a cilinder surface; but maybe you just find something arround there / kindly :)
Code:
(
tool Z offset = tool center, not tool ege
run it easy at 1st, step-by-step, be aware of where it
is going before pushing cycle start; approach is directly
at cut diameter, there is no feeding among X-
carefull with Z clearance, because is a little big than
usual, and maybe it will colide with the tailstock ... in such a
case, pls let me now if you need a modified clearance; don't modify it
directly inside the program, because it corelates with the number of
loops, and, instead of 7, there will be a decimal number, that has to
be calculated
)
V1 = tool rpm
V2 = feed_g95 for the helix
V5 = feed_g95 for final retreat among X
V3 = target diameter
V4 = turret post
( * )
G00 X_up Z_rigth
T+V4*101
M110
SB=V1 M13 ( M08 )
VZSHZ = - [ 3.9370 - 3.8898 ] + [ 7 - 2 * VPAI ]
G00 X=V3 Z0 C0 M15/M16 ( choose how the helix wraps arround )
CALL OSUB Q7
X_above_part G90 F=V5 ( don't rush this movement, also don't use G00, because tool may cut during it's way out; tool retreat/disengage is different when C axis is used )
M12
M109
G00 X_up Z_rigth T+V4*100 VZSHZ = 0
OSUB
G01 Z-0.5315 C359.999 G91 G95 F=SQRT((360*0.5315*360*0.5315+500*360*500*360)/(360*0.5315*360*0.5315+V3*360*VPAI*V3*360*VPAI))*V2
RTS
