Okuma lathe post problem

[Leif Johnson from MICO Inc]

Hello. I updated the MPLOSP7C post from V9. That is the only mill / turn post for the OSP that I have available. It doesn't output any Zs & the Xs are all wrong. I uploaded a zip2go named Okuma_post_problem.Z2G to the lathe folder on the FTP site. I have no idea what the problem is, please help!

 

Thanks,

Leif

[DavidB]

Leif,

There is no MCX file in your zipped file?

 

Is your toolpath a C-axis or a turn?

[Leif Johnson from MICO Inc]

Isn't there bad_okuma_post.MCX?

[Leif Johnson from MICO Inc]

I will redo.

[DavidB]

This is your z2go file.

[Leif Johnson from MICO Inc]

try Okuma_post_problem_3.Z2G

 

Thanks

Leif

[DavidB]

You are correct there no Z moves and the X values are backwards X-1. instead of X1.

 

Code from your file

N3

( TOOL - 3 OFFSET - 3 )

( LFINISH NVLCR-163D_VPGR-331 INSERT - VPGR-331 )

( Okuma L370 )

G0 X20. Z20.

G50 S1750

VZSHZ=V1

G97 T0303 S1750 M42 M3 M87 M8

G0 X.04 Z0.

G96 S500

G95 G1 X0. F.005

G3 X-.0913 R.0457

G1 X-.5313

G2 X-1. R.2344 -- SHOULD BE X1.

G1 ---MISSING Z MOVE

G3 X-1.5313 R.2657

G1 X-2.

X-1.9717

M9

G0 X20. Z20.

M05

M02

 

Is this the first time you have run theis in MCX?

Your values are radial too not diameter?

[DavidB]

This is your file with my Okuma post..

$T.MIN%

( T )

(DRAWING NUMBER - ?)

(DRAWING ISSUE - ?)

(PROGRAM ISSUE - ?)

(PROGRAM CREATED ON THE - 07-10-06 11:07 )

( )

(OPERATION NO. ?)

(SET Z ZERO TO FRONT FACE OF PART)

(WHICH IS ??MM FROM JAWS/COLLET FACE)

( )

N100 M109 (C AXIS AUTO CLAMPING OFF )

N110 G50 S1750

( TOOL - 3 OFFSET - 3 )

( LFINISH NVLCR-163D_VPGR-331 INSERT - VPGR-331 )

N120 G0 X21.6535 Z7.874

N130 T0303

N140 G96 S500 M03

N150 G0 X0. Z.02 M08

N160 G95 G1 Z0. F.005

N170 X1.9087

N180 G3 X2. Z-.0457 K-.0457

N190 G1 Z-.2656

N200 G2 X2.4688 Z-.5 I.2344

N210 G1 X3.4688

N220 G3 X4. Z-.7657 K-.2657

N230 G1 Z-1.

N240 X4.0283 Z-.9859

N250 M09

N260 G0 X21.6535 Z7.874

N270 M05

N280 M02

%%

[Leif Johnson from MICO Inc]

Are you using the 2 axis post that came with V9? What happened during the convertion? When I use the mill / turn post in V9, everything is great, less than great after converting.

 

Thanks

Leif

[DavidB]

Your machine def does not look right.

 

All my MCX post are updated from V9 and I have not had a problem.

 

Did you use your V9 posts to also create the Machine and control defs when you used the update post c-hook?

[Leif Johnson from MICO Inc]

Yes, I've done all of mine that way. Something really got hosed, just not sure what & how.

[Leif Johnson from MICO Inc]

I just ran the update post again with the same results

[Leif Johnson from MICO Inc]

Any ideas as to what I need to change? We just got the machine & I had been using the 2 axis post. I will need this post to work so I can use some live tools. I did a beyond compare of the V9 & the updates X post. The following is the only major differences other than the $:

 

linktolvar$ : 1 #Associate X tolerance variables to V9- variable?

linkplnvar$ : 1 #Associate X plane specific variables to V9- variable?

linklvar$ : 1 #Associate X lathe specific variables to V9- variable?

cant_tlchng$ : 1 #Ignore cantext entry on move with tlchng_aft?

 

 

If I select the version X - 2 axis post with this machine def, everything is fine. Any help is greatly appreciated.

 

Thanks

Leif

[Leif Johnson from MICO Inc]

Bump

[DavidB]

Leif,

In MCX open a Lathe Machine def from the standard machines that came with MCX.

 

Now from the drop down menu "Machine Type" goto machine def, edit controll def, Post processer.

Add files and add your post to this Machine def close and save. Now in the toolpath manager, files, Machine, Edit you can select which post you want to use. Select your post and see what you get with a standard Machine and Control def but with your post.

[Leif Johnson from MICO Inc]

I tried that with the same results. I think it is the post. I will try again.

[DavidB]

Leif,

It will not work.

 

I tried it.

What the problem is your post is the

# Description : GENERIC OKUMA /W LAP3 CYCLES & C-AXIS SUPPORT

# Mill/Turn : YES

This post will not do a turning toolpath you need to use...

 

# Description : GENERIC 2 AXIS OKUMA /W LAP3 CYCLES

# Mill/Turn : NO

 

For turning ops use the above post and your post for your C and Y axis work.

 

Okuma

Okuma

[Leif Johnson from MICO Inc]

Did Dave have a mill / turn post available? Maybe I will have to use my 2 axis post alittle longer.

[Leif Johnson from MICO Inc]

Are you still posting 2 separate programs & pasting together?

[DavidB]

quote:

---

Are you still posting 2 separate programs & pasting together?

---

Yes

 

There is there is NO Okuma post that will do canned cycles for turning and also C and Y axis toolpaths.

 

So I have a machine def for Okuma turning and a machine def for Okuma Milling.

[Leif Johnson from MICO Inc]

Do you use the lap cycles? I generally long code everything. It's too bad there isn't a mill / turn post. Hopefully someone is working on one.

[DavidB]

Yes I use Lap cycles that's why I need a turning post and a milling post.

[Greg Williams]

David,

 

I am sure that Inhouse can do a post

[DavidB]

In-house said it would be a merge of the two posts.

I'll check my emails tomorrow and add there reply here it was awhile ago now.

 

How's the new job working out for you Greg?

[DavidB]

Re-email from In-house

 

quote:

---

You can sort of merge your working mill and working lathe post together by using m in place of p for mill and l in place of p for lathe in the postblock names

 

psof

 

becomes lsof for lathe ops, msof for mill

 

you can build a composite post that way, that smashes your two post together.

 

Let me know if you'd like a quote. I'm sorry we don't have anything that directly suits your machine.

---