Okuma MA-400VA Horizontal f99999

[Brian L.]

Hello All, New memember, first post here. Sorry it has to be a question about, of all things, a post.

 

I'm a student at the Rochester Institute of Technology and we have several Okuma machines at our disposal. We have been running a converted and modified version of a mc9 post that never worked well to begin with.

 

I am using Mastercam X3 with the mpmaster_okuma_horizontal.mmd

and what i think is a modified version of

mpmaster_okuma.pst

mpmaster_okuma.control

 

I am attempting to utilize our machine's B axis to its fullest potential and I cannot seem to get code that works perfectly.

 

Issue 1

feed rates are set to f99999 within a drilling cycle the correct feed rates are read from the tool setup in mastercam.

 

Issue 2

After calling G15 H2 (correctly calling the work ofset)

Just before the first Z move it calls G56 H0 canceling the tool offset I think?

 

Other than those problems the code looks ok. It properly orients the B axis (after i changed the machine def.) and the code looks good.

 

I'm sure this is something relatively simple but i have very little understanding of posts. Any help is greatly appreciated.

 

-Brian-

[gcode]

If this post is an updated X2 mpmaster see the

X2 X3 update sticky thread 4th from the top of the

page

[Brian L.]

Well I feel kindof silly for not reading that post before asking. Thank you for pointing that out. I have edited my post accordingly and I will try it first thing in the morning.

 

Any thoughts on the other problem with the z offsets?

[35K chipper]

Brian ,

here is a snip from one of my Okumas G56 is the tool length for that tool.

 

{NEXT TOOL ACTIVE WITH / OFF}

{PGM Z MAX Z.3}

{PGM Z MIN Z-.6449}

G0G90G80G40G17G94

N2

IF [VATOL EQ 2] N78

M121

T2M6

M9

N78

{.500 3FL SE VIPER STLTH }

{RF SPINE}

G131J2I0

{MAX Z.3}

{MIN Z-.315}

/T7 {IS THE NEXT TOOL}

G0G90G15H5X.901Y-5.4535S30000M3

G56H2Z.3M8 <<<<<<<<<<<<<<<<<<<<<<<<<

G4F3.

Z.15

G1Z.071F1400.

X11.149

Y-5.9455

X.901

Y-5.4535

Z.021

X11.149

Y-5.9455

X.901

Y-5.4535

Z-.029

X11.149

Y-5.9455

X.901

G0Z.3

{RF BACK}

G131J2I0

 

hope this helps

 

35k

[Brian L.]

Yep thats the line im referring to in mine it just says

 

Nxxx G56 H0 Z2.3

 

The tool call prior to this called T2

Subsequent tools are called correctly and so do the different work offsets. However immediately before the first Z move as i showed, it calls H0 instead of the H(X) for the tool I'm using.

[gcode]

Check the settings on the Tools page

of the Control Definition

[Colin Gilchrist]

The reason it is giving you an H0 is that your tool definition has a zero for the offset number.

 

There are some options in the Control Definition file to force the Diameter and Height offset numbers to match the tool number.

 

Once you set the height offset number for all your tools, the G56 Hxx lines will come out with the H code matching the T number...

 

HTH,

[35K chipper]

Brian,

save a copy of your post then look for these lines.

 

pstartabs # First Move in contour {forced Absolute}

if opcode$ = three, pstartxyz

pxycalc

 

*sgcode, pabs, pwcs, *xabs, *yabs, *speed, *spdlon, prange, pcan, e$

"G56", *tlngno$, *zabs, pcoolon, e$

 

the call *tlngno$ may be missing or the * is missing.

 

35k

[Brian L.]

I opened it in notepad and searched several different ways and I could not locate those statements. The tlngno$ exists in several places some with * and some without.

 

I couldn't find the statement:

pstartabs #

[Colin Gilchrist]

It isn't a post problem!!!!

 

Your post is doing exactly what you've told it to do.

 

Give me a "G56", and use the H offset that is listed on the Tool Definition Parameters page. You just need to set your tool parameters to have the diameter and length offsets match the tool number...

[Brian L.]

GREAT!!! Got it guys, turns out i'm just noobish when it comes to programming. Setting the offset numbers in the tool files fixed it immediately.

 

Unfortunately, after modifying the post according to the stick recommended by gcode, it still outputs F99999.

 

Here is the most recent output, not that it tells you much...

 

code:

---

 (MCX FILE  - C:USERSBRIANDOWNLOADSBRACKETS PAIR.MCX)

(POST - MPMASTER_OKUMA)

(MATERIAL - ALUMINUM INCH - 2024)

(PROGRAM - BRACKETS PAIR.MIN)

(DATE - JUN-11-2009)

(TIME - 9:19 PM)

(POST DEV - IN-HOUSE SOLUTIONS)

(T3 - 1/2 FLAT ENDMILL - H3 - D3 - D0.5000")

(T1 - 1.22" KEYSEAT CUTTER - H1 - D1 - D1.2200")

(T2 - 1/4 CENTERDRILL - H2 - D2 - D0.2500")

(T6 - 25/64 DRILL - H6 - D6 - D0.3906")

(T5 - 1/4 FLAT ENDMILL - H5 - D5 - D0.2500")

(T4 - 1/4 BALL ENDMILL - H4 - D4 - D0.2500" - R0.1250")

(OVERALL MAX - Z3.2)

(OVERALL MIN - Z.2)

N100 G00 G17 G20 G40 G80 G90

N110 G30 P1

N120 G116 T3 ( 1/2 FLAT ENDMILL)

N130 (MAX - Z2.537)

N140 (MIN - Z.7)

N150 G15 H2

N160 G00 G17 G90 B0. X-1.9999 Y-3.7501 S12224 M03

N170 G56 H3 Z2.537 T1

N180 Z2.037

N190 G94 G01 Z1.8462 F999999.

N200 Y-1.9999

N210 Y-1.7095

N220 G02 X-1.8463 Y-1.5559 I.1536 J0.

N230 X-1.6928 Y-1.7095 I0. J-.1536

---

 

[ 06-11-2009, 09:20 PM: Message edited by: Brian L. ]

[35K chipper]

Brian,

Colin is right about your settings. sorry i took you in the wrong direction. when you said they were version 9 posts that didnt work well.

never thought to ask what your d and h values were for the tool. my bad

 

35k

[Brian L.]

No biggie I figured it was something simple that i missed. I was so used to 9 its hard adjusting.

 

Still confused about the feedrate thing, ive googled a bunch and havent turned up any more info.

 

Oh, and Colin, I know a couple of people that just started at Boeing within the past couple of weeks. Not sure what dept. they are with though.

 

[ 06-11-2009, 10:15 PM: Message edited by: Brian L. ]

[Colin Gilchrist]

Hey good deal Brian.

 

For your feedrate problem, I think you have some parameter settings in the post that are wrong...

 

Check this thread, and then check for the sections in your post that read these parameters and make the changes that are listed...

 

If you need help you can email me a copy of your post and I'll take a look tomorrow. I'm off work on Fridays so it won't be a problem...

 

Thanks,

[Brian L.]

Thanks Colin, this morning i took a look at the post again and realized that i had misread the description in that thread. I read the "was XXXX" to be the change to be made not the other way around. I changed the parameters and everything works perfectly.

 

Thank you all for your help. If anyone needs a working post/machine def. for x2 or x3 for an okuma MA-400HA let me know....

[Greg Williams]

You could always just turn off the tool length number

 

G00 G17 G40 G80 G90

G30 P32

IF [VTLCN EQ 1] N1(SPINDLE TOOL CHECK)

T1 (12. FLAT END MILL CRB)

M6

N1 (SPINDLE TOOL JUMP)

S2600 M03

G15 H1

G00 G90 X-61.1909 Y-12.8588

G56 H=VTLCN Z50.

Z47.5

G01 Z37.5 F300.

[Greg Williams]

Or use a custom tool change macro to set the H and D

 

 

I use this one

 

OTCK(GET NOMINATED TOOL G116)

IF [PT EQ EMPTY] NERR

IF [PT EQ VTLCN] NEND

IF [PT EQ VNTOL] NM6

IF [VNTOL EQ 0] NCT

M64

NCT T=PT

NM6 M6

NEND G56 H=PT D=PT

GOTO NRTS

NERR M63

M6

NRTS RTS

RTS

 

Register OTCK to G116 in custom G and M codes

 

The Gcode will be

 

G00 G17 G21 G40 G80 G90

G30 P1

M404

(SWARF NEW TOOLPATH)

(TOOLPLANE NAME - TOP)

G116 T5 ( 16. FLAT ENDMILL)

M27 (C-AXIS UNLOCK)

M11 (A-AXIS UNLOCK)

G15 H1

G0 G17 G90 G94 A-19.1423 C58.4052.

S8000 M3

X50 Y50

Z100

[Brian L.]

Thanks guys, i just ran a program today with the edited post, everything works perfectly. Now i just need to figure out how to use the canned text and make that work properly.

 

I want to turn on Block Delete for only two operations but when i turn it on it puts optional block delete on for the entire program. Is there any way to do this without using subprograms?

[Colin Gilchrist]

You need to use these settings:

 

For the first op, "Block delete on" & "With".

 

For the second op, "Block delete on" & "With", then add another canned text set to; "Block delete off" & "After".

 

So what you are doing is enabling block delete for the first and second ops, then turning it "off" after the second operation.

 

This is how it is done most of the time, depending on how your post is setup. If you try my suggestion above and still get block delete on the whole program do this:

 

Set your "Bld on" and "With" for the 1st and 2nd op. In all the other operations, set "bld off" and "with"...

 

HTH,

[Brian L.]

Ah... i understand. I did not know i needed to turn it off after I was done with it. Worked like a charm. Thank you once again Colin.

[Colin Gilchrist]

Anytime man, glad you got it working.