What's new
What's new

Okuma LB-3000EXII programming C-axis on while milling

vibco

Plastic
Joined
May 23, 2019
Hello All,
I am trying to write a program that will allow me to use a ball end mill to cut an inverted radius on the face of a shaft..4375 Rivet Set v1.jpg


So I am trying to turn the spindle at a constant speed (M03 ) while also having the the live tooling spindle on.

I could easily do this cut with a small bore bar with the correct clearance, but I figured I would try something new and use both C and live tooling to cut the profile.

This is what I currently have for code. I am getting alarm 2702-01 "SPDL. command during C-axis connect A side"
I was told that M152 should allow me to do this. I have tried to change the layout of this code, but still get the same alarms. (don't mind my speeds and feed, I need to change those later). Thanks for the help!!


M110
M146
G94
SB=2445 M13
N0600 G97 S20.0 M03 M152 M08
N0601 G00 X0.7353 Z0.6 T080808
(N0602 G96 S300)
N0603 G87 N0604
N0604 G81
N0605 G00 X0.814
N0606 G01 Z0.5 G41 F3.82 ("/MIN)
N0607 Z0.095
N0608 G03 X0 Z-0.312 I-0.407
N0609 G40 G01 X0.5 Z-0.2726
N0610 G80
N0611 G97 S2292 M05 M09
N0612 G00 Z0.6
N0613 X20 Z20
M109
M153
G95
N0614 M01
 
If I'm reading that right, your M110 is turning on the C-axis, and you can't give a spindle command with the C axis active. Your M152 is just allowing you to run the live tool and the spindle at the same time. Since the feature is centerline, I would take the M110 and M109 out completely.

Edit: I also can't think of a single good reason to do this.

Edit x2: Yeah, honestly this is a terrible idea. Take a video when you run it, I'd love to see it.
 
I’m not familiar with this machine but when using a c axis I’m programming it with a feed rate in degrees per minute
 
Haters, i do it every now and again to make the same detail, best success was in 300m steel

you're not going to be using c axis, but rather m spindle interlock release

M-Tool Spindle Interlock Release Function (Optional) - Okuma OSP-P200L Programming Manual [Page 174] | ManualsLib

I recommend roughing with a drill and boring out as much material as you can

you can program it as a standard boring pass with the radius of the endmill equal to TNR.

then you flip parameters around a little
lathe spindle rpm = feed rate --- 2 sfm = 24 IPM
feed rate= step over .02 ipr = .02 step over
lathe spindle direction= climb or conventional

it does tend to leave a little bit of a mottled finish but you can follow it up with a micro 100 QPR tool for a light skim cut

also i have asked for a variance before to allow a small drill point at the center of the sphere which increases tool life greatly regardless of approach
 
I have roughed out a shape already. I just need to do the finish pass with the end mill.

I cant get the M152/M153 to allow me to run the program.
 
Okay, just took out M110 and M146 and started the block with M153 and the part came out mint.
Thanks for the help everyone.
 
Haters, i do it every now and again to make the same detail, best success was in 300m steel

When you go to a grocery store, and ask the produce person what herb to use in your marinara. And he says Oregano, but you were thinking Mint leaves. It doesn't make him a "Hater". We're adults here, we don't even know what a hater is. This isn't Facesuk. If you'd like to be a participant---don't do that.

R
 
Haters, i do it every now and again to make the same detail, best success was in 300m steel

you're not going to be using c axis, but rather m spindle interlock release

M-Tool Spindle Interlock Release Function (Optional) - Okuma OSP-P200L Programming Manual [Page 174] | ManualsLib

I recommend roughing with a drill and boring out as much material as you can

you can program it as a standard boring pass with the radius of the endmill equal to TNR.

then you flip parameters around a little
lathe spindle rpm = feed rate --- 2 sfm = 24 IPM
feed rate= step over .02 ipr = .02 step over
lathe spindle direction= climb or conventional

it does tend to leave a little bit of a mottled finish but you can follow it up with a micro 100 QPR tool for a light skim cut

also i have asked for a variance before to allow a small drill point at the center of the sphere which increases tool life greatly regardless of approach
Ha! Next thing you know people will be asking why the headstock rotates on a grinding machine!!! 😂
 








 
Back
Top