Okuma LB200-MY lathe programming help

[Philcott]

We have the above mentioned lathe and I need some help figuring out what the code needs to look like to run some C axis face milling on this.

 

First of all, we have a lot of programs written to run on our fanuc controls and we would like (if possible) to be able to tweak the code to run on the Okuma. If we could change the G113 to G137 or something like that it would be great but I have a feeling it won't be as easy as that.

 

Below is a sampling of the code I use now. The X value is the diametrical distance along the horizontal axis (X on a mill) and the C is the radial distance along the vertical axis (Y on a mill).

 

What I need to know (we are new with this machine and I don't have much for sample code with explanations) is when programming with G137 where do I get my values for X and Y? From there I can start working on some post mods to get me going.

 

 

The machine has a Y axis but for now I want to try and get this conversion going

 

Any help would be much appreciated.

 

 

G0 X4.0161 Z.25

M8

G112

G1 X-.3536 C2.0002 F100.

Z.05

Z-.25 F6.42

G41 X-.1768 C1.9119 F40.

G3 X0. C1.8753 L.125

G2 X.8186 C1.6243 L.4593

X1.8444 C.2121 L6.1562

X1.8925 C0. L.9462

X.3694 C-.9281 L.9462

G3 X.3402 C-.9607 L.0437

X.3904 C-1.0003 L.0437

G2 X.9185 C-1.416 L.4592

X0. C-1.8752 L.4592

X-.8186 C-1.6243 L.4592

X-1.8444 C-.2121 L6.1562

X-1.8925 C0. L.9462

X-.3694 C.9281 L.9462

G3 X-.3402 C.9607 L.0437

X-.3904 C1.0003 L.0437

G2 X-.9185 C1.416 L.4592

X0. C1.8753 L.4592

X.1984 C1.8644 L.4593

G3 X.2524 C1.8615 L.125

X.3868 C1.8811 L.125

G1 G40 X.5976 C1.9483

Z.25 F100.

G113

 

 

I have a .Z2G profile that we have used on our fanuc controls I can send if someone wants to try and help.

[Mr. M]

You can send it to me if you like, on the Okumas they use G137 and then G101,102,103 vs G01,G02,G03

If using Cordinate conversion, you program the face op just as you would on a mill as far as X,Y positions. I can send you some sample programs if you like

(edited to add information)

[Philcott]

PM sent. Forgot to ask for email addy.

[Mr. M]

PM sent, here is a quick sample of Code for a 2" square move using the Cordinate Conversion function

G137 C0
G00 X1 Y1
M13
G01 Z-0.25 F152.8 M147
G101 Y-1 F30.56 M146
X-1
Y1
X1
G00 Z0.12 M147
M146
G136

[Philcott]

That bit looks simple enough. You will see from the file I sent that the part will need to use cutter comp as well as G102 and G103's throughout the profile.

[Mr. M]

Email sent with code, let me know what else you need

[Philcott]

Now we're getting some where. The code (with a couple housekeeping tweeks) ran the profile.

 

I at least now now what I need the post to output for me. Now begins the most un-enjoyable task of messing with a post to get what I need.

 

Email sent

[T_MALENA]

Thats exactly how I do it here... G137/G136 & G101,102 & 103 and let the machine crunch the math to rotate c-axis. Works out to (I think) a smoother cut in turn a faster cut.

[Mr. M]

Yes, it converts the feed from IPM to DPM vs doing inverse time.

[Philcott]

I hear talk about a MplmasterOkuma post. Is that post a downloadable and then modifiable post? My inbox awaits any and all replies.

[Mick]

The MPLOkuma Inhouse post is a cost post afaik. You will need to talk to Inhouse about that. I had an older version a few years back, and from memory it was really good.

 

CNC Sofware have some nice Okuma posts. Talk to your reseller about those.

[Philcott]

The MPLOkuma Inhouse post is a cost post afaik.

 

Bummer.