Broaching on a Mazak Lathe

[SpecialtyMfg.]

We have a Mazak 250 that we have attempted to broach on. However, when trying to program using a Mazak manual process, the machine won't feed without the spindle turning. Does anyone know a work around for this? Or which parameter possibly to change?

 

Thanks

[Guest]

I know on other machines you have to be in IPM mode and not IPR

[htm01]

i have a program for our mazak integrex that a guy from mazak did for us, he said he modified it from lathe prog

 

we ended up buying a broaching head and get custom inserts made

 

 

this is EIA for Integrex, maybe you can modify. if not shoot me your email address and i can give you contact info

 

<9998B>(SHAPING O.D. MALE KEY)

#1  = #1      (A)(SIDE CLEARANCE ON EACH STROKE)

#3  = #3      ©(C AXIS POSITION TO CENTER THE HOLE TO X AXIS)

#6  = #6      (K)(DIMENSION ACROSS OD TO SIDE OF MALE KEy)

#7  = #7      (D)(DIAMETER OF OD)

#8  = #8      (E)(END OF KEY SLOT IN Z AXIS)

#9  = #9      (F)(SHAPING FEED RATE IN IPM)

#18 = #18     ®(REMOVAL AMOUNT PER PASS)

#19 = #19     (S)(START OF KEY SLOT IN Z AXIS)

#20 = #20     (T)(NUMBER OF TIMES TO REPEAT LAST PASS)

#32=[#6-[#7/2]]*2  (CALCULATE X STARTING POINT) 

#33=#7             (PASS INCREMENTER - END AT OD)

 

G109 L1                       (SELECT UPPER TURRET)

G00 G17 G20 G40 G80 G90

G91 G00 G28 X0.

G28 Y0. Z0.

G10.9 X1                      (X DIA MODE)

 

G90 G0 X#32 Z#19 M200

C#3 M8

G97 M5

N1 G1 X#32 Z#19 F300.

G1 Z#8  F#9

G91

X#1

G90

G1 Z#19 F300.

#32=#32-#18-#18        

IF[#32GT#33]GOTO1     

N2 #20=#20-1

G1 X#32 Z#19 F300.

G1 Z#8  F#9

G91

X#1

G90

G1 Z#19 F300.

IF[#20GT0]GOTO2

 

M9

G10.9 X0                       (X RDAIUS MODE)

G0 Z.1

G91 G28 X0. Y0.

G28 Z0.

M99

%

[mkd]

From personal experience, if you buy a broach from Dumont they will supply a really cool macro program available for various controls. It will probably have all the needed codes setup already.

 sorry I don't have the specific answer.

[Watcher]

http://integrexmachinist.com/forums/index.php?action=vthread&forum=1&topic=353&page=1

 

Horn tools are great too!

[Allan]

Simple as:

 

G98 Feed per minute

G99 Feed per rev

 

The posted macro also does not contain the G98 on line N1 so without the G98 it would just sit there.

 

 

[SlaveCam]

OT but broaching on our lathe makes the Z-axis servo motor so hot we have to apply air pressure to it to avoid excess temperature alarm.

[htm01]

Simple as:

 

G98 Feed per minute

G99 Feed per rev

 

The posted macro also does not contain the G98 on line N1 so without the G98 it would just sit there.

must have been active already because it ran as is

[Allan]

must have been active already because it ran as is

 

I was thinking about that could be the M200 looks after it.

Easy way to tell... single block and see if the modal value G98/G99 change after the line.

On second thought does the Mazak have a screen that shows? it should.

[htm01]

I was thinking about that could be the M200 looks after it.

Easy way to tell... single block and see if the modal value G98/G99 change after the line.

On second thought does the Mazak have a screen that shows? it should.

we don't use that program anymore we bought a broaching head went from one insert /10 parts to 3 months on same insert