c-axis programming lathe
Hello;
I am looking for a few sample programs using the c-axis feature for the lathe.
The equipment I will be using is Yama seiki ga-2000 series
with a fanuc Oi TB controller
I am looking for milling,drilling and tapping examples.
I am also wondering about the difference in using either the c or h for controlling the chuck rotation?
my email is
pjmorand@hotmail.com
Thank you
Similar Threads:
You would be better off looking at your manuals for prog examples as each machine maker seems to use different codes for activating live tooling
other than this drill tapping and basic milling are the same as turning G01 for feed you feed per rev or meters per min. you are just dealing with X, Z in a slightly different way.
C usually is absolute degrees H is incremental move.
ST
Thats the problem I am having the maker did not include any examples.
The m codes are ,
m18 c-axis cancel
m19 c-axis on
m29 rigid tapping
m73 revolve tool forward
m74 reverse
m75 stop
H and c as you mentioned
What G-codes are involved other than g97,g98
Thanks
G87 AND G88 are drilling and tapping with the -X- axis on the od of a part
If you can ENVISION it I can make it
Thank you King,
Got any sample programs?
don't know if this will work for you but this is from a fanuc control
q has to be reapeted on every line
r is an incremental value from x start point
remember x is diametrical and y is radial
substitute G88 for the tap. g88 is already rigid tap mode
N6(3/64 DIA TIN COATED COBALT DRILL )
G30U0W0
M35( milling mode)
M90( unclamp c axis)
G0G40G80G97G98
G0G54T0606
/M33S2491
M110 ( interferance check)
M8
G0C0.Z-.1Y.445
X.46
G87C0.X-.425Q300R-.025M89F3.5
C120.R0500Q300M89
C240.Q300R0500M89
G80X1.0
C0.M90
G28V0
G28H0
G30U0M35
M5
M1
If you can ENVISION it I can make it
Thank you King!
I will give it a whirl!
Paul
This is a recent Drill and Tap program I used on our Leadwell CNC with Fanuc OiTB Control. We don't have B-Axis to cross-mill and can only Mill, Drill and Tap on the centerline in the Z direction only. Remember when milling, your finish depth will be in diameter. I tried to add notes where possible. I hope this helps.
[THERE ARE THREE MILLED FLATS FOR N3...ONE EACH AT 180 DEG., 0.0 DEG, AND 270 DEG.]
N3 (MILL CYLINDER FLAT)
(TOOL 1.250 OD END MILL)
G50 S3500
T0303 G54
M60
M5
M90
M191
G97 S424 M95
G98
G0 G28 H0
G0 C-180.
G0 Z0.75
X1.7500 M8
G0 X1.0635
G1 Z-1.3 F3.4 (First pass @C180.0)
G0 X1.7500
G0 Z0.75
G0 X0.752 (Finish Dia.{depth})
G1 Z-1.3 (Final pass @ C180.0)
G0 X2.7500
Z0.75
(MILL SENSOR FLAT)
G98
G0 C0.
G0 Z0.75
X2.7500
G0 X1.0500 (Finish Dia. {Depth})
G1F6.79
G1Z-1.3 F5.0 (Final Pass @C0.0)
G0X2.7500
Z0.75
(MILL AIR HOLE FLAT)
G98
G0 C270.
G0 Z0.75
X2.7500
G0 X1.352 (Finish Dia. {Depth})
G1F6.79
G1Z-0.700 F6.0 (Final pass @C270.0)
G0X2.7500
Z0.75
M9
M95
G0 X8.
G0 Z4.
M1
[THERE ARE THREE CROSS-DRILLED HOLES FOR N7...2 ON C0.0 @ Z-0.25 AND Z-0.846 AND 1 ON C270.0 @ Z-0.846]
N7 (#29 CROSS DRILLED HOLES)
(TOOL .136 CROSS DRILL - MAIN)
G50 S3500
T0505 G54
M59
M90 (C-Axis1 Mode On)
G0G28H0 (Home C-Axis)
G28C0.0 (C-Axis to 0.0)
G0X1.475
G0Z-0.25
G97G98S3000M94
M8
G87X0.125C0.0Z-0.25Q2500F4.0M35 (Drill Peck cycle @C0.0)
Z-0.846Q2500 (2nd hole on C0.0 @ Z-0.856)
G80
M36 (C-Axis1 Unclamp)
G0X1.452
G87X0.125Z-0.846C270.F4.0M35 (Drill Peck cycle @C270.0)
G80
M36 (C-Axis1 unclamp)
M95 (Spindle Stop)
M91 (C-Axis1 Mode OFF)
M9
G0X8.0
G0Z4.0
M1
[THERE ARE THREE CROSS-TAPPED HOLES FOR N8...2 ON C0.0 @ Z-0.25 AND Z-0.846 AND 1 ON C270.0 @ Z-0.846]
N8 (8-32 TAP 1)
(TOOL 8-32 TAP - CROSS)
G50S3500
T0707G54
M59
M90 (C-Axis1 Mode On)
G0X1.5
G0Z0.25C0.0
Z-0.25
X1.65
M65S721 (PMC-Axis Control ON)
G188U-0.375Z-0.250C0.0R0.3F0.03125S721D1.05 (Tapping cycle @C0.0)
Z-0.846 (2nd Tapped hole on C0.0 @ Z-0.846)
M66 (PMC-Axis control OFF)
M36 (C_Axis1 Unclamp)
G0X1.959
C270.0 (Rotate C-Axis to C270.0)
M65S721 (PMC-Axis Control ON)
G188U-0.375Z-0.846C270.R0.30F0.03125S721D1.352 (Tapping cycle @C270.0)
M66 (PMC-Axis control OFF)
M36 (C_Axis1 Unclamp)
M91 (C-Axis1 Mode OFF)
M9
G0X8.0
G0Z4.0
M1
Thank you jbird68!
Paul
Hi CNC king ,I know it's a long shot as this post I'm replying to is really old but I have to mill this shape (external profile) and am proper stuck using c axis face milling ,I'm working a cmz turn mill 32i fanuc controls ,Originally Posted by cnc-king
Would love some advice ,just hope I can attach the photo of the part ,I have a 10mm dia vrx to rough and a 8mm dia vrx to finish ,both 5 flute coated carbide ,please please please lol ,
If you can't see the attachment then maybe you can forward an email address and I can send it to you ,I'm on my own in the workshop so under quite a bit of pressure to sort this.
Many thanks
Simon
Re: c-axis programming lathe
Hello Simon,
If your control has the Polar Coordinate Interpolation option, then your part is simple to program. If not, then you really need a CAM system to generate a tool path made up of small linear moves.
To determine if your control has the Polar Interpolation function, create a short program as follows:
G112 (or G12.1)
M00
G113 (or G13.)
M30
If the control accepts G112 (or G12.1) without raising a p/s 010 alarm, then your control has the option. If no alarm results, run the above program to the end to ensure Polar Interpolation is cancelled with G113 (or G13.1). If a p/s 010 alarm results, go no further and delete the program, as in this case it will have been confirmed that the control does not have the Polar Interpolation option.
Regards,
Bill
Re: c-axis programming lathe
Where are you now guys! you've been talking about c axis 20 years ago! after 20 years I'm again searching for that content. you are very great. hope to see this message in health!
Posting Permissions
Reply with Quote