Makino A99 Post

[Odin]

WE have a Makino MCB 1210 HMC and we just got a Makino A99 HMC. Will the Makino 1210 post work on the Makino A99? I have it post to machine, but it keeps saying improper G code. I'm not sure what to do.

I couldn't attach the post

Thanks

[Guest]

Which G code is the one causing the error?

 

Until you know that it's tough to say

[Odin]

I think its G43. here is the first ten lines of the program.

%

O0000(SC4 HELPER)

G17G40G49G80

(T37 2.0 HELIMILL .063 CR )

M741(CONVEYOR ON)

G0G90G40G54X-7.3568Y-.5108S955M3

G43H37Z2.

G05P10000

Z.1

G1Z.065F100.

 

 

The machine alarms out on the highlighted line.

 

Thanks

[Guest]

Take out the G5P10000

 

Betting you don't have the highspeed option

[Odin]

ill give that a try, but im pretty sure that we have look ahead.

[Odin]

That worked,

Thanks

[Guest]

[Guest]

You have look-ahed, you just don't have HPCC.

[Odin]

Yeah, are sister company failed to tell us that the sent us the wrong machine, the machine we got doesn't have the SGI. they are pulling the board out as I'm typing. I also have another program error. it is 003 too many digits. I cant figure that one out,. in the post under the format statements it has this...

 

# Format statements - n=nonmodal, l=leading, t=trailing, i=inc, d=delta

# --------------------------------------------------------------------------

#Default english/metric position format statements

fs2 1 0.7 0.6 #Decimal, absolute, 7 place, default for initialize (

fs2 2 0.4 0.3 #Decimal, absolute, 4/3 place

fs2 3 0.4 0.3d #Decimal, delta, 4/3 place

#Common format statements

fs2 4 1 0 1 0 #Integer, not leading

fs2 5 2 0 2 0l #Integer, force two leading

fs2 6 3 0 3 0l #Integer, force three leading

fs2 7 4 0 4 0l #Integer, force four leading

fs2 9 0.1 0.1 #Decimal, absolute, 1 place

fs2 10 0.2 0.2 #Decimal, absolute, 2 place

fs2 11 0.3 0.3 #Decimal, absolute, 3 place

fs2 12 0.4 0.4 #Decimal, absolute, 4 place

fs2 13 0.5 0.5 #Decimal, absolute, 5 place

fs2 14 0.3 0.3d #Decimal, delta, 3 place

fs2 15 0.2 0.1 #Decimal, absolute, 2/1 place (feedrate)

fs2 16 1 0 1 0n #Integer, forced output

fs2 17 0.2 0.3 #Decimal, absolute, 2/3 place (tapping feedrate)

 

I'm not sure what to do! is it a post problem or a machine parameter issue?

TIA

[Guess_who]

Yes, they are formatted inside the post. You should see a line like this "

 

fmt "C" 2 P9990_C

 

This is formatting the variable P9990_C to an absolute decimal 4/3

 

Find the variable you need to change and see what it is formatting it to. It's is as simple as changing that number in the fmt statement.

[Odin]

There is no fmt "C" P9990_C in the post anywhere, this is thefmt lines in the post,

 

 

# Toolchange / NC output Variable Formats

# --------------------------------------------------------------------------

fmt "T" 4 t$ #Tool Number

fmt "T" 4 first_tool$ #First Tool Used

fmt "T" 4 next_tool$ #Next Tool Used

fmt "D" 4 tloffno$ #Diameter Offset Number

fmt "H" 4 tlngno$ #Length Offset Number

fmt "G" 4 g_wcs #WCS G address

fmt "P" 4 p_wcs #WCS P address

fmt "S" 4 speed #Spindle Speed

fmt "M" 4 gear #Gear range

# --------------------------------------------------------------------------

fmt "N" 4 n$ #Sequence number

fmt "X" 2 xabs #X position output

fmt "Y" 2 yabs #Y position output

fmt "Z" 2 zabs #Z position output

fmt "X" 3 xinc #X position output

fmt "Y" 3 yinc #Y position output

fmt "Z" 3 zinc #Z position output

fmt "B" 11 cabs #C axis position

fmt "B" 14 cinc #C axis position

fmt "B" 4 indx_out #Index position

fmt "R" 14 rt_cinc #C axis position, G68

fmt "I" 3 i$ #Arc center description in X

fmt "J" 3 j$ #Arc center description in Y

fmt "K" 3 k$ #Arc center description in Z

fmt "R" 2 arcrad$ #Arc Radius

fmt "F" 15 feed #Feedrate

fmt "P" 11 dwell$ #Dwell

fmt "M" 5 cantext$ #Canned text

fmt "P" 4 dtloffno

fmt "R" 1 mr1$

#CNC<<MSG-ERROR(498)>> The format statement number is not defined (default to 1)

#CNC<<MSG-ERROR(497)>> The format statement number is not defined (default to 1)

# --------------------------------------------------------------------------

#Move comment (pound) to output colon with program numbers

fmt "O" 7 progno$ #Program number

#fmt ":" 7 progno$ #Program number

fmt "O" 7 main_prg_no$ #Program number

#fmt ":" 7 main_prg_no$ #Program number

fmt "O" 7 sub_prg_no$ #Program number

#fmt ":" 7 sub_prg_no$ #Program number

fmt "X" 2 sub_trnsx$ #Rotation point

fmt "Y" 2 sub_trnsy$ #Rotation point

fmt "Z" 2 sub_trnsz$ #Rotation point

# --------------------------------------------------------------------------

fmt "Q" 2 peck1$ #First peck increment (positive)

fmt "I" 2 peck2$

fmt "Q" 2 shftdrl$ #Fine bore tool shift

fmt "R" 2 refht_a #Reference height

fmt "R" 2 refht_i #Reference height

# --------------------------------------------------------------------------

fmt "T" 4 tnote # Note format

fmt " DIA. OFF. - " 4 toffnote # Note format

fmt " LEN. - " 4 tlngnote # Note format

fmt " DIA. - " 1 tldia$ # Note format

[Odin]

The machine is alarming out when it goes to do the output feed move (in highspeed waterline) , I unchecked the box in mastercam and it works, it just slow .

[Guess_who]

The fmt "C" P9990_C, is just an example. I'm not sure what variable you want to change. post your code, and point us to what word is incorrect.

[Odin]

I got it. on the high speed waterline program, the machine didn't like the 4 digit feed output move, I changed it to 200.0 on MasterCam and it worked just fine.

Thanks for all the help fellas!!