Makino A51 ???

[melmar]

Good day to all

 

Our shop has recently purchased a Makino A51 HMC with the Pro 5 control and we are having some difficulties with the HSM. The program it is running ran fine in a 2003 Kitamura

and also in a 2006 Robodrill Mate. The programmed feedrate is 500 I.P.M. and though never quite reached in either machine due to size of part it did get close. The same program

in the Makino tops out at 60 I.P.M. and stays there ? I dont know if there is something we are overlooking in the machine control or if it is in Mastercams post ? Any ideas ?

 

Thanks

[Odin]

CHeck your machine dynamics, OP feedrate limits, and axis feed rate limits in your General machine parameters in mastercam's machine def. See if they are set to low for the makino. We had the same problem when we Used our post from our mori seiki for our Makino S56. Also check your output feedrate in your highspeed toolpath program parameter.

[melmar]

Thanks for the info.

I checked all that you mentioned. Everything appears to be in order. I am however a little sketchy on what the machine dynamics should read when I get into the feedrate smoothing and cornering.

But gave that part of it my best educated guess. When it comes to the Makino and the Pro 5 do you know if we should use a G5.1 or a G5 P10000 or I believe there is even a G8 ?

[Odin]

On our S56 with the Pro5 we use G05 P10000 for look ahead. Same as our Makino MCB1210 with Pro 3 we use The G05 P10000 and the end of the program we use G05P0 to end the look ahead. Something like this

 

O0000

G17G40G49G80

(T31 .250 DIE SINKER )

G0G90G40G54X5.7528Y2.1259S12500M3

G43H31Z2.

G05P10000

Z.0999

~

~

~

~

Z-.4903

G0Z2.

G05P0

G91G30Z0.M5

G53G49

M30

[Odin]

Melmar,

Did you get everything lined out?

[melmar]

Had'nt been able to try anything til this morning. Had to get some parts out as is, and in the mean time had to get the reps out here with continual coolant / filter issues.

Any way, we tried the G05 P10000 and get an improper G code alarm ? The G5.1 will run it, but way slow as previously mentioned. Any more ideas I'm all ears. I'm also sending

program to dealer to see if it will run in their floor model.

Thanks again

[BenK]

Is that a roughing code you are running? We have Makino horizontals here and the fast feedrates aren't an issue.

[Odin]

Check your output feed move in your program. If your using the high speed toolpaths it could affect your speeds.

We had a problem with that before when we was using HST on a slow machine.

[melmar]

Using Mastercam X4, couldnt find my " output feed move "? - BenK, are you guys also using G05 P10000 ?

[Joe788]

I thought the Pro 3 and 5 controls had simple M-codes to control this stuff, like M251 for finishing, M252 for semi finishing, M253 for SUPER RADICAL or something along those lines?

[BenK]

No g05 is part of the super GI function and we don't have that option. For roughing code we use g4p0 it makes the machine cut really fast but you will need to leave some extra stock to finish. If you want you can send me the code in question and I can take a look at it tonight.

 

I thought the Pro 3 and 5 controls had simple M-codes to control this stuff, like M251 for finishing, M252 for semi finishing, M253 for SUPER RADICAL or something along those lines?

 

Yes you are correct, M255 is radical mode for use when roughing. If your machine defaults to M251 or M252 it will cut a little slower than if it defaults to M255. Your best bet is to just put the codes in the program.

[melmar]

Just a thanks to all that cared. Problem solved.

 

A simple case of over thinking the processs. I had to take a step backwards but long story short we had to loosen up some deviation tolerances and allow more arc code instead of linear.

[Odin]

Glad you got it figured out!