Okuma post radius output

[chris m]

I searched for this but couldn't find anything; I'm trying to (slowly) enter into the world of (simple) post modifications and I figured I'd start with a post that works pretty close now. The MPLOKUMA post works pretty well but I get an "R" instead of an "L" for circular interpolation; how can I change this?

 

Thanks

 

C

[Allan Brown]

search for arcrad and can the format statement?

[chris m]

OK Dave; not really understanding what you're saying

 

The arcrad statement looks like this:

 

fmt R 2 arcrad #Arc Radius

 

Should I change it to something else? Should it be this?

 

fmt L 2 arcrad #Arc Radius

 

Please advise what you mean

 

------------------------------------

 

Let the record show that I tried this and it didn't do what I thought it might

 

------------------------------------

 

C

 

[ 04-08-2003, 01:01 PM: Message edited by: chris m ]

[chris m]

OK

 

I think it is working correctly now; is what I did correct?

 

I added string definitions for slrad and slrminus using "L" instead of "R" to mimic those for srad and srminus. I then changed the parcrad call to look for slrad and srminus instead of srad and srminus.

 

I posted an operation and it seems to work OK.

 

Does that mean what I did was right or is something waiting to bite me in the butt?

 

Thanks

 

C

[Allan Brown]

Forgot about the srad srminus things. Otherwise you did the right thing in the format statement. After that your slrad stuff was all on target. Way to go!

[chris m]

Dave

 

Thanks

 

I changed the format statement back to the original iteration, though; should I re-modify it to have an "L" instead of an "R"?

 

It seems to work OK now so I'm hesitant to screw with it, but I don't want to be bitten down the road either.

 

C

[Mick]

Chris,

 

What kind of Okuma control is it? We've got three at work (OSP7000L, OSP700L and U100M)

Do you use LAP cycles? I'd like to implement them into the post a bit better, and make them easier to use. Maybe we could trade notes

 

Cheers,

 

Mike

[chris m]

Mike

 

We have a few:

 

(4) 5020L (Cadet LNC8 lathe)

(2) U10M (ESV machining center)

(1) U100L (LT-15M)

(4) E100L (Captain L370 lathe)

 

Right now we're using Mastercam's .nc files for the geometry data only and pasting it into our standardized program format but I'm trying to (slowly) get to the point where we can post and run.

 

The post that I've been customizing a little bit is just the MPLOKUMA that ships with Mastercam, which appears to "really" be a Fanuc post that has some formatting changes so that it spits Okuma-like code.

 

The header says that it supports LAP3, but below it says that it doesn't support canned cycles

 

For right now longhand code is OK, though it is a pain in the butt if you want to change a stock-on amount or depth-of-cut quickly at the machine. I would like to get into LAP down the road but I'm not really sure how a post handles that. I've seen posts that do output LAP cycles but I'm not really sure how they work.

 

If I see something I like I'll be sure to let you know; please do the same.

 

C

[Roger Martin from CNC Software]

quote:

---

The post that I've been customizing a little bit is just the MPLOKUMA that ships with Mastercam

---

Which MC version CD are were talking here ?

 

The MPLOKUMA.PST that was on the v9.0 CD did LAP3 cycles, and other (threading & drilling) canned cycles

[chris m]

I believe it was the V8.1 post that I started with:

quote:

---

# Post Name : MPLOKUMA

# Product : LATHE

# Machine Name : OKUMA

# Control Name : OSP7000

# Description : GENERIC 2 AXIS OKUMA /W LAP3 CYCLES

# Associated Post : NONE

# Mill/Turn : NO

# 4-axis/Axis subs. : NO

# 5-axis : NO

# Subprograms : NO

# Canned Cycles : NO

# Executable : MPL v8.1

---

You'll see above why I was confused with this:

 

quote:

---

The header says that it supports LAP3, but below it says that it doesn't support canned cycles

---

I'm not doing anything very sophisticated with it so if I would be better off using the V9 post as a baseline it wouldn't be a big deal to start over and make the same changes; what should I do?

 

C

 

[ 04-09-2003, 03:56 PM: Message edited by: chris m ]

[Roger Martin from CNC Software]

If you are going to twekk a post for your use -

It's ALWAYS a good idea to make sure you are starting out with the lastest version available.

[Mick]

Roger,

 

That is correct, the MPLOSP post does support LAP3 cycles, but in a round about way. I modified an old version, which outputs the LAP format using the misc. reals.

It would be nice to be able to choose the Rough Turn toolpath, input depths of cut, stock etc, and then have a checkbox type scenario to allow a "Canned Cycle" output. I've often wondered if it was feasible, both for turning and facing. Much like the choices you have when threading, between Canned, Box, Longhand etc.

I get asked by quite a few people about this, and it would certainly be appealing

 

Cheers,

 

Mike