M19 question for Doosan Mynx 7500

[JeremyV]

We've recently got a new machine about a year ago - a Doosan Mynx 7500...

 

I'm wondering if anyone runs their machines in a certain way or there is a requirement for a M19 in the program to reduce wear + tear on the spindle?

 

As in....   the code below is how we run it:

 

(T3 = .375 SPT DRILL )
N40 (SPOT .531 THRU HOLES)
N50 G00 G91 G28 Z0.
N60 T3
N70 M6
N80 S6000 M03
N90 G00 G54 G90 X-1.9375 Y-.95
N100 G43 H3 Z4. M08 T13
N110 G94
N120 G98 G82 Z-.08 R.1 P400 F50.
N130 X1.9375
N140 G80
N150 M09
N160 G00 G91 G28 Z0.0
N170 M01

 

 

During tool change, the spindle revs up to the previous RPM then orientates automatically.

 

The machinist has been putting M19 in the program as shown below:

(T3 = .375 SPT DRILL )
N40 (SPOT .531 THRU HOLES)
N50 G00 G91 G28 Z0.
N60 T3
N70 M6
N80 S6000 M03
N90 G00 G54 G90 X-1.9375 Y-.95
N100 G43 H3 Z4. M08 T13
N110 G94
N120 G98 G82 Z-.08 R.1 P400 F50.
N130 X1.9375
N140 G80
N150 M09
N160 G00 G91 G28 Z0.0 M19
N170 M01

 

 

What I'm wondering is if both of the two quotes above will damage the spindle or?

 

If a M05 is required to follow immediately after M09, then whats what we'll have to do if we want the spindle to last without issues.

[#Rekd™]

M19 locks the rotation of the spindle does it not?

[JeremyV]

M19 locks the rotation of the spindle does it not?

It does... and orientates for tool change.

 

I wonder if it does more harm than good...

[jlw™]

I have never heard of spindle orientation doing any harm whatsoever. It does this regardless of M19 or not.

 

I bet on that machine you can even orient to a given angle. Try something like M19S180 or M19S1800 to go to 180° from TC angle. I use this for the occasional sneaky broach path.

[The Cathedral]

Just modify the tool change macro to work how you want. The very first code we have in there is M05, so whenever an M6 is called, the spindle stops.

[JeremyV]

Just modify the tool change macro to work how you want. The very first code we have in there is M05, so whenever an M6 is called, the spindle stops.

Would you happen to know where I can find that?

[The Cathedral]

Depends on your control. I'm assuming you have a Fanuc. The tool change macro is a 9000 series program, so you'll have to change the parameters that let you access those programs. Set parameter 3202.4 to 1 to unlock them, and 3202.6 to 1 to see the programs (when 3202.6 is set to 0, the program runs discreetly, which is why you never see it on the screen.) Once you do that, you can find the program number in your directory and change it to what you need.

 

And if you screw anything up, that's all on you and I take no responsibility, so tread carefully.

[Newbeeee™]

Seriously, if you don't know where or how to find the toolchange macro, I'd stay WELL away.

Do as your machinist is doing - change your post processor to output M19 instead of M5 and the machine will stop in the orientated position and seamlessly toolchange.

[JeremyV]

Yea - all on me, I get that....  hah

 

I did try the above mention and it wouldn't behave the way I wanted it to behave.  Like it wasn't reading the M05 or something?

 

Is there a certain spot in the program where it needs to be?

[Newbeeee™]

You have it in the same position as we do and every machine I've known works okay like this.

As it goes home for the toolchange, the spindle slows and stops in the correct position and immediately toolchanges.

No additional orientating, it just toolchanges (or sits there in the correct orientated position if you haven't called a toolchange and just sent the spindle home).

What does the machine do when you run the prog with the M19?

Does it go home and then spin and then stop and orientate, and then toolchange?

If it does, it is the way your toolchange macro (program) is written.

if the machine is only 12 months old, I'd get your dealer to change the macro.

[JeremyV]

It goes home, stops at M01 when M01 is enabled, then after cycle start it spins and then stop and orientate, and then toolchange?

 

if the machine is only 12 months old, I'd get your dealer to change the macro.

I fixed the first line description to what it does now without M19.

 

my answer to the last question in the quote is yes - it was provided as default

 

We've had the machine for 11 months - I'd presume it is a little older than that, but not much.

 

 

However when I add M19 in the program itself, the spindle stops and orientates itself before M01.  At tool change, the spindle does not rev up due to the M19 being in the NC program.  Without the M19, the spindle behaves as stated in the quote.  I think a M05 would be better than M19 in the NC program itself.  Modifying the post file is the easy part tho.

[The Cathedral]

All you need is the M05, before the M01.

 

The M01 is basically just "pausing" the machine, and as soon as you hit cycle start it goes back to what it was doing. If the spindle was running before hand, it will start up after. If it's stopped, it stays stopped.

 

An M19 should already be buried in the tool change macro so you won't have to worry about that (if it's not, your MTB was drunk on the job and you'd better start demanding some free tech support.)

 

I would put the M05 on the same line as the G28 to save cycle time; if you don't you'll lose a few seconds every tool change.

[civiceg]

MP master has the M05 before the G91G28Z0. It really is the post to use for FANUC. 

[absolute technologies]

On Mori machines there is a keep relay that allows M-codes to be performed during movement or after the movement so I have a M19 on the G28 line so that by the time Z-axis gets home the spindle is oriented and ready for a tool change. There is no need for a M5 as the M19 stops the spindle then orients all in one motion so it's probably faster not to have an M5. This saves about a second per tool change you might want to check to see if Doosan has something similar.  I've never heard of M19 causing wear and tear on a machine. At M19 essentially there is current going to the spindle servo motor to hold the spindle position and it takes very little power to hold that position.

 

Cheers!

Len Dye

[PAnderson]

No need for the M19 as it is already in the tool change program. When you do a tool change, watch what macro program it runs. Usually 9006. Yes, there is a keep relay like Len Dye says. I don't have a Mynx book in front of me so can't tell you which one. There is a blue book in the electrical cabinet door that has all of the keep relays for that machine. As for the M19 outside of the tool change program, no, it will not hurt it.

 

Paul Anderson

Applications Engineer

Doosan Machine Tools

973-618-2457

[The Cathedral]

I don't believe he was worried about the M19 wearing the spindle. Rather, the spindle stopping for the M01, then restarting and immediately stopping again for the tool change.

[THEE THAINZ™]

Put an M5 above your M09 line then add the M19 to the G28 line if it does not orientate automatically. If your spindle locks by the use of an detent you will cause wear to the locking mechanism by putting the brake on while the spindle is still at RPM.

[JeremyV]

Thx for all the information guys lol...

 

I added a M05 on the G28 line.... there really is no loss of time with the M05 in program.

 

Boss thinks its a Kaizen and wanted me to fill out a form, I told him its not.  The amount of idiots I work with cause me to scratch my head in disgust. ( story for another day)