New Makino A51 NX on the way

[Bob W.]

Well, I finally pulled the trigger on a horizontal and ordered a new Makino A51 NX that should be arriving in a few weeks. I have only owned and run Haas machines in the past and I am hoping that this is a step up in quality and performance :-) The options I added were Super GI.4 high speed machining, tool and part probes, Data center, and a few Fanuc memory options. Now the real work begins...

 

I want to get this machine up and running ASAP and I would like to implement modular fixturing for the tombstones, which I will be ordering this week. Anyone have any advice for a strategy that works? Any links to articles etc...? The next major item is getting a post processor situated. What is the best way to go about that? I'm not even sure where to start. Is there a solid Makino horizontal post out there, or should I start from scratch with the MPFAN? My Haas posts have been evolving over the years and I pretty much have them dialed in exactly how I want them with utilization of the misc integers and such. How is the pallet switch handled in programming a horizontal? Is the M code inserted in the program via manual entry or is it usually done at the machine?

 

Any help or advice will be appreciated! I can hardly wait to get this sucker in the door.

[BenK]

We just add the M60 before the end of the program to switch the pallet.

 

If I'm running one pallet:

 

M60

M0 (CHANGE PARTS)

M60

M99

 

 

 

For both pallets it would just be:

 

M60

M99

 

This way you don't have to keep hitting cycle start every time.

 

You can set it up to read what pallet is in the machine by using some goto and Macro's so it will know what program to run. Monday I will see if I can share how we do it, I should be able to but I better ask.

 

 

You will love that machine and it will be hard to go back and run a Haas after running the Makino.

[dforsythe]

I like to keep everything modular. All of the pallets I designed have a 2 x 2 grid of .750 c/b .200 deep with a ½-13 helicoil thread in the middle. This allows us to go from vertical to horizontal and the 5 axis with the same fixtures ( there are size limitations). Im also a big fan of dovetail fixtures. I know it add an extra operation, but for running lights out and pure work holding rigidity it’s a price I’m happy to pay. You can also make rail fixtures that hold the part with set screws tuned on a lathe from the side. we also use a lot of ball lock tooling so anytime a pallet has room we add that pattern in as well. As far as vise and cluster towers I really like toolex although we do use chic here. Nice machine. I’m sure you will love it. if you do all of your tooling up front its quick and easy to use down the road. We design and build the majority of ours. It’s not cheaper, but we get exactly what we want.

 

for MC we use the MPmaster with a few modes for tool number and d # along with the proper high speed call outs. your makino should always use H1, D1 for all tools.....i think, its been a while. we also use the dynamic work cord macro. ( we NEVER program from c/l ) unless its a part on a mushroom fixture rotating on the center of a pallet. our other cam system output the g10's in the prg.

 

(UNPROVEN PROGRAM)

(MPMASTER HAAS EC-500)

(1XXXX_RB.OP1.NC)

(POST - HAAS EC-500)

(DATE - DEC-09-2011)

(TIME - 3:14 PM)

(****G10 INFORMATION START****)

G90

M98 P9002

G10 L2 P1 X.005 Y9.321. Z8.225

G65 P9018 A54. B90. C55.

G65 P9018 A54. B270. C56.

(****G10 INFORMATION END****)

M01

M31

(T59 - AJX_1500_3FL_INSERT_CUTTER)

(T51 - HANITA .500 4F EM 1.25 LOC .030 CR 1.3 PRO)

(T52 - 3/8" 4F FLAT CAR EM 1.0 LOC RD .36 RL 1.1 PRO 1.150)

(T53 - HANITA .500 4F EM 060 CR 1.25 LOC 1.3 PRO)

(T54 - HANITA 1/4" 4F CAR BNEM .750 LOC .030 CR RD .230 RL 1.05 PRO 1.1)

(T55 - 1/2" X 120 DEG. HSS SPOT DRILL)

(T56 - #5 HSS DRILL STUB LENGTH)

(T57 - .215 HSS REAMER )

(T58 - 1/8" X 90DEG CARBIDE CHMF MILL 2F PRO 1.1)

(OVERALL MAX - Z10.)

(OVERALL MIN - Z-1.1617)

G00 G17 G20 G40 G80 G90

G91 G28 Z0.

(FACE TOP +.010)

N59 T59 M06 (AJX_1500_3FL_INSERT_CUTTER)

G90G10L12P#3026R0

[Bob W.]

your makino should always use H1, D1 for all tools...

 

Could you elaborate on this a little?

 

One idea I had that CNC Apps guy (James) mentioned a while back was having the post store tool and offset numbers in macro variables such as #500 and having the H and D values reference that same variable. I was also thinking of setting the tool diameter in another variable so the tool setter could reference this and use the same variable when setting lengths on large diameter tools such as saws, etc... I would like to automate the tool setting process using macros so if the machine loads a tool and the length offset for that tool is set to zero in the machine it would automatically set the tool using the setter. Of course this depends on the operator setting the offsets to zero when the tools are removed from the machine. Basically all tools would just be loaded into the machine (with a value of 0.0 for all length and diameter offsets) and on the first cycle the machine would set all of the tools automatically. Anyone use this sort of strategy? I have heard that the learning curve is pretty steep initially.

[Bob W.]

we NEVER program from c/l

 

Why not? I am curious because I had planned on having the first four work offsets correspond the the pallet top and center line with 54 being A0, 55 = A90, 56 = A180 and 57 = A270. Then the other offsets would be utility offsets that would be set per the job. Can work offsets be locked on the Fanuc control? What about tool offsets?

 

Another item I am not sure about is the machine has 60 tools that fit in 60 pockets. If the control can store 400 offsets how does the tool loading/ setting process go? With the Haas I have always had the tool and offset numbers match.

 

 

Thanks for the input, it is very informative.

[dforsythe]

Could you elaborate on this a little?

 

One idea I had that CNC Apps guy (James) mentioned a while back was having the post store tool and offset numbers in macro variables such as #500 and having the H and D values reference that same variable. I was also thinking of setting the tool diameter in another variable so the tool setter could reference this and use the same variable when setting lengths on large diameter tools such as saws, etc... I would like to automate the tool setting process using macros so if the machine loads a tool and the length offset for that tool is set to zero in the machine it would automatically set the tool using the setter. Of course this depends on the operator setting the offsets to zero when the tools are removed from the machine. Basically all tools would just be loaded into the machine (with a value of 0.0 for all length and diameter offsets) and on the first cycle the machine would set all of the tools automatically. Anyone use this sort of strategy? I have heard that the learning curve is pretty steep initially.

 

on a makino it might be H1, D9 for eveything. i dont think you would need to go thru the trouble of storing a variable as 99% of cnc machines automatically store this already ( haas = #3026 hitachi = #4400 ect) its been a long time since i programmed for a makino, but i think the control acounts for this and the tool in the spindal reference pulls the propper h and d storing them in the H1 and D9 location all in the background. we have mostly haas and func here so our haas post spits out #3026 anytime there is a D or H callout. this prevents someone from making a mistake.

 

when using resident tooling you may have to comp a tool -.001, but the same tool is used on another op or pallet that might not need it. setting these localy will allow you to dial in each part without having to adjust the tool comp hard #

 

agian, this is just what i think i remember about the makino

 

 

G00 Z10.

M05

G91 G28 Z0.

G90G10L12P#3026R0

M01

(ROUGH LEFT OVER STOCK)

N51 T51 M06 (HANITA .500 4F EM 1.25 LOC .030 CR 1.3 PRO)

G90G10L12P#3026R0********************************************************writes the comp calue local*****************************************

(MAX - Z10.)

(MIN - Z-1.04)

(TOOLPATH - ROUGH REST PASSES)

(STOCK LEFT ON WALLS = .035)

(STOCK LEFT ON FLOORS = .035)

M11 (UNLOCK)

G00 G17 G90 G54 A0. X.5763 Y.477 S2139 M03

M10 (LOCK)

G43 H#3026 Z10. T52

M08

Z.4401

G94 G01 Y.4796 Z.0457 F11.12

Y.499 Z.0121

Y.5326 Z-.0073

Y.552 Z-.0099

Y.6536 F22.25

G02 X.4828 Y.6671 I.0481 J.6622

*******************************************

X-1.0175 Y-3.6133 I-.0402 J.5296

X-1.0986 Y-3.5534 I.3481 J.5567

X-1.2064 Y-3.4202 I.3424 J.3875

X-1.275 Y-3.1789 I.4796 J.2667

X-1.2178 Y-2.9187 I.5271 J.0206

G03 X-1.2724 Y-2.7505 I-.1114 J.0568

G01 G40 X-1.3838 Y-2.6937

Z-.94 F11.12

G00 Z10.

M09

M05

G91 G28 Z0.

G90G10L12P#3026R0 *********************************************** clears cutter comp value*************************************************

M01

[dforsythe]

Why not? I am curious because I had planned on having the first four work offsets correspond the the pallet top and center line with 54 being A0, 55 = A90, 56 = A180 and 57 = A270. Then the other offsets would be utility offsets that would be set per the job. Can work offsets be locked on the Fanuc control? What about tool offsets?

 

Another item I am not sure about is the machine has 60 tools that fit in 60 pockets. If the control can store 400 offsets how does the tool loading/ setting process go? With the Haas I have always had the tool and offset numbers match.

 

 

Thanks for the input, it is very informative.

 

 

Programming from c/l is one of those things that gets debated often. Im the supervisor here, so I program and have my guys program for local work coordinates. I just like the flexibility of being able to run a job in a offset kurt vise one day and on a c/l chic tower the next with zero re-programming. You can make precision parts with a quality setup programming from c/l. I have done it and seen it done a lot. Its just something I don’t care for when you are using a probe to double set secondary local work cord in the middle of a program. I love the fact the if an operator needs to shift a feature -.0023 on the side of apart all he does is edit the macro call. Or shift the Z on G56 +.0007 for a blend as shown below.

 

 

(****G10 INFORMATION START****)

 

G90

 

M98 P9002

 

G10 L2 P1 X2.5. Y13.2. Z14.753

 

G65 P9018 A54. B90. C55. X-.0025

 

G65 P9018 A54. B220. C56. Z.0007

 

(****G10 INFORMATION END****)

 

 

 

 

as far as 60 tools. thats not much. you could prob have 30 residents and leave 29 open for special tools and one for the probe. take extra time looking at the kind of work you do before setting the tool list. i group them by order i comonly use them 1-10 insert cutters 11-20 are end mills the all the common spot, drill and taps we use. the rest are all open for special tools.

 

 

[MotorCityMinion]

"54 being A0, 55 = A90, 56 = A180 and 57 = A270."

 

This, IMO, defeats the purpose of programming from CL. (my personal preference back in the days of Horizontals and engine blocks) True C/L being XZ requires only G54 for all rotational values. This require that the parts be located repeatedly at a fixed location known prior to programming the job. This works best with large , single parts that get fixtured or windowed fixtures. Program the A axis on a vertical, and most folks don't change a WPC just because A45. was called up. Same here.

 

Multiple parts on a Tombstone may be different of course, but with a good set-up using C/L and good planning C/l will work here as well.

 

Sure, some on the fly set-ups will be faster just clamping the part down anywhere and establishing a New wpc.

 

Now, G54 is pallet 1, G55 for pallet 2 and so on. X and Z will remain the same in all the WPC's if you do program from C/L just like YZ would remain constant on a A-axis.

[Bob W.]

This, IMO, defeats the purpose of programming from CL

 

My thinking was that I will often have different jobs on each side of a tombstone so I could change a job's location just by changing the work offset. If job A was to be on the front of the tombstone it would be run at G54. If it was on side B it would be run on G55, at least that is my thinking. Often I will string programs together with a master program and M98 commands using a variable for the work offsets. Here is an example:

 

#500=54

M98 P1

M01

#500=55

M98 P2

M1

#500=56

M98 P3

M30

 

Then all work offset calls in the program are edited and changed to G#500 so program 1 would be run on G54, etc... With a change of one variable I can change where the program is run so I could put any job on any side of a tombstone and simply change a macro variable to accomplish that. I think it would work for well fixtured, repeat work. I am pretty new to this and have zero experience with horizontals though. It is hard to plan for this stuff with no experience. I have to add that this strategy has worked fantastic on my Haas machines and it is very flexible.

[YoDoug®]

Why not? I am curious because I had planned on having the first four work offsets correspond the the pallet top and center line with 54 being A0, 55 = A90, 56 = A180 and 57 = A270. Then the other offsets would be utility offsets that would be set per the job. Can work offsets be locked on the Fanuc control? What about tool offsets?

 

Another item I am not sure about is the machine has 60 tools that fit in 60 pockets. If the control can store 400 offsets how does the tool loading/ setting process go? With the Haas I have always had the tool and offset numbers match.

 

 

Thanks for the input, it is very informative.

 

I use a macro that knows the x-z machine position of the rotation of the Baxis and use that to calculate new work offsets for any rotation. That way you just touch off a part or locating surface of a fixture one time. Call up the macro for each index of the part and your offsets are automatically populated.

 

 

 

[YoDoug®]

Here is the code for the rotation macro for anyone interested. Fanuc Macro B, I am working on an Okuma version and should have it finished soon. Just change the #541 and #542 for your machines X-Z machine coordinate of rotation center of B. Also there are two inputs to incrementally shift the new offset after it is calculated. It works for both G54-G59 and extended offsets. It could probably use a few more checks to look for empty inputs.

O9910
IF[#23GT49]GOTO50
IF[#23GE1]GOTO200
IF[#23EQ#0]GOTO3000

N50#100=[#23-53]

(W = WORK OFFSET TO BE USED FOR CALC)
(R = NEW WORK OFFSET NUMBER)
(B = INDEX AMOUNT)
(X = INC TO NEW X ZERO AFTER ROTATION)
(Z = INC TO NEW Z ZERO AFTER ROTATION)

#540=-19.682 (MACHINE POS X ROTATION)
#541=-42.13 (MACHINE POS Z ROTATION)

#542=#[5201+[#100*20]] (STORE CURRENT X OFFSET FOR CALC)
#543=#[5203+[#100*20]] (STORE CURRENT Z OFFSET FOR CALC)


#544=[#542-#540](DELTA X)
#545=[#543-#541] (DELTA Z)

#546=SQRT[[#544*#544]+[#545*#545]] (HYP FOR CALC)

#547=[ASIN[#544/#546]] (START DEG FOR CALC)

#548=[#547+-#2] (CACL DEG)

#549=[sIN[#548]*#546] (NEW DELTA X)
#550=[COS[#548]*#546] (NEW DELTA Z)

#551=[#549+#540] (NEW X OFFSET)
#552=[#550+#541] (NEW Z OFFSET)

IF[#18GT49]GOTO2
IF[#18GE1]GOTO20
IF[#18EQ#0]GOTO3000

M99

N200#100=[#23]

(W = WORK OFFSET TO BE USED FOR CALC)
(R = NEW WORK OFFSET NUMBER)
(B = INDEX AMOUNT)
(X = INC TO NEW X ZERO AFTER ROTATION)
(Z = INC TO NEW Z ZERO AFTER ROTATION)

#540=-19.682 (MACHINE POS X ROTATION)
#541=-42.13 (MACHINE POS Z ROTATION)

#542=#[6981+[#100*20]](STORE CURRENT X OFFSET FOR CALC)
#543=#[6983+[#100*20]](STORE CURRENT Z OFFSET FOR CALC)


#544=[#542-#540](DELTA X)
#545=[#543-#541] (DELTA Z)

#546=SQRT[[#544*#544]+[#545*#545]] (HYP FOR CALC)

#547=[ASIN[#544/#546]] (START DEG FOR CALC)

#548=[#547+-#2] (CACL DEG)

#549=[sIN[#548]*#546] (NEW DELTA X)
#550=[COS[#548]*#546] (NEW DELTA Z)

#551=[#549+#540] (NEW X OFFSET)
#552=[#550+#541] (NEW Z OFFSET)

IF[#18GT49]GOTO2
IF[#18GE1]GOTO20
IF[#18EQ#0]GOTO3000

N2
G90G10L2P[#18-53.]X#551Z#552B#2
G91G10L2P[#18-53.]X#24Z#26
M99

N20
G90G10L20P#18X#551Z#552B#2
G91G10L20P#18X#24Z#26
M99
N3000#3006=[(NO WORK OFFSET CHECK G65 LINE)]  

[BenK]

I use a macro that knows the x-z machine position of the rotation of the Baxis and use that to calculate new work offsets for any rotation. That way you just touch off a part or locating surface of a fixture one time. Call up the macro for each index of the part and your offsets are automatically populated.

 

This is how we do it as well. One of the big advantages to the horizontal is the 4th axis and only using one offset is the way to go. If you get a chance go to the Makino Macro training, they should go through things like this. I haven't been to the training yet but both of the other programmers have been and form what they say it is well worth it.

 

 

 

 

For the tool numbers we use H1 D1 for every tool. We have a tool offset program that wrights all the offsets to the machines that we just call up at the beginning of our main program. This way we can keep tools setup without having to remeasure them when we put them back into the machine.

 

O1234(TOOL OFFSET PROGRAM)

(assign tool numbers)

M53

T1(pot number)

#701=#4120 (#710=tool 1)

T2

#702=#4120

M37

(too offsets)

M53

T[#701]

S43750(LENGTH OF TOOL)(43750=4.3750)

M54 (makes next line a negative value)

S00005(DIAMETER VALUE)(00005=0.0005)

T[#702]

S000

S000

M37

M99

[Chris Rizzo]

WOW Bob that's cool! I've got a very good friend down in Bend that programs for a two-machine A51 cell. He comes up here frequently. I'd be happy to put you in touch.

 

hth

[Bob W.]

WOW Bob that's cool! I've got a very good friend down in Bend that programs for a two-machine A51 cell. He comes up here frequently. I'd be happy to put you in touch.

 

hth

 

Sure, I'd love to hear what he has to say. I definitely need to rethink how I will be setting things up. There is some great advice in here.

[MotorCityMinion]

Sure are quite a few strategies listed here. I never got into the production/quantity side of things. My suggestion was pretty much an out of the box technique. When I did load more than one part on a tombstone or fixture, it was usually 4 to 6 operations of the same part positioned differently, never the same operation performed at 4 or 6 locations.

 

For angle plates, I've used the gussets at 90 and 270 to hold parts. A shorter tombstone with a fixture plate on the top (looking down at Y-) can yield additional workspace as well.