[Brian FRF]

Got this machine in here 500v model, with yasnac mx1 controller.

Just been slow going learning how this machine wants to talk to me. Bit different gcode, and navigating to the offset tables, entry etc has been slow. So what Im wondering is if someone familiar with these machines wants to give a bit of a crash course in entry of info into the controller. If you are willing, shoot me a message. Be happy to call on my dime, and figure out some compensation as well.

Also, is there a way to show the list of programs currently in the computer. Figure I could use the method of reverse figuring the programs to help me as well.

[PixMan]

Going back about 10 years, I worked for a small company to program, set-up, operate and service a machine exactly like that. It's been a while, but I could probably help.

Where are you located? I'm in central MA. If close enough I could help in person much better than by telephone.

[Brian FRF]

Going back about 10 years, I worked for a small company to program, set-up, operate and service a machine exactly like that. It's been a while, but I could probably help.

Where are you located? I'm in central MA. If close enough I could help in person much better than by telephone.

Hmm, I think youre only 1500 miles away then!

Im getting closer as we speak, still trying to figure out how to enter fixture offsets, tool length offsets, and if its even possible to display all the programs saved in memory (what if I need all the memory, and need to erase all of them?)

[dcoupar]

G54 XYZ, etc. go into Settings (see attached).

[Brian FRF]

Found that spreadsheet, but Im having a time trying to find where to plug in the numbers? If I start at parameters it starts at 6001, so Im sure Im in the wrong place.

[maz43]

The program list should appear if you go to alarm mode and cursor up.
There should also be a timer in there.
Yaskawa.com has free pdf manuals for the mx1,2 and3.
Work offsets should be able to be input via mdi using G10Q2P#x#y#z#.
P1 for g54, P2 for g55,etc.
Not sure about the MX1, but on MX2&3 If you set shifts via parameter you must first change setting 6219 t0 1.
After changing shift parameters be sure to put 6219 back to 0.

[Brian FRF]

Well getting somewhere. Just setting up a 2 hole peck drill cycle to play with.

Odd behaviors Im getting:
using a g43 and h1 (-2.0) and that works for my z offset. However at the start of the program, the tool goes down past part zero, in rapid, by ~2", rapids back to r plane (.1), then proceeds to normal drilling cycle.

After drilling the last hole, Ive got g80, g40, g52, then g0z0, to get the tool back to the tool change position. Im getting z overtraveling, trying to go higher than the tool change.

As for g54, and the offsets, I just did a g92x0y0 to zero the part. Main reason, I went to the 6516, in settings, and I can change the numbers, but no decimal points? Maybe it doesnt use them, and just uses 6 places?

Ill try messing with 6219, and see where I get too.

Im definately getting closer, just taking a bit!

I downloaded the yasnac manual, printed it out, and bound in a binder. And Ive got the operators manual that came with the matsuura. Little bit more step by step. Im just looking for the "spoon fed" directions!

[maz43]

Use G49 Z0 to cancel H offset.
There are no decimal points in the work zero parameters.
Example:290001 is 29.0001.
If you use G10Q2 P# X#Y#Z# and enter it via mdi, you can use decimals and you don't have to mess with parameters when setting work shifts.
P1 for G54, P2 for G55, etc.
When calling g43 use G43H1Z1.
That should stop 1 inch above the part.
If you are using the measure button to set tools remember that there is a parameter setting for gage block size.

Good luck!

[Brian FRF]

Ooops, meant to say I do have a g49 after the last hole, and Im still overtraveling z?

[stevo1]

Brian…Maz43 is right on with the G43 call. In order to establish the G43 there must be a Z move in the line. When you put G43Z-2H(). That is why the machine moved -2”. As Maz said if you put Z1 it will move 1” above. You must be careful of using G49Z0 because depending on where Z0 is set up to on your machine it could be interfering with your part. If Z0 is table top the tool will move to table top.

A way to avoid this all together is I code into all of my macro’s the proper Z’s for G43 and G49. When G43 is given if you were to make the Z in that line the “current machine position” minus the “tool offset” then your machine will not move in the G43 line. With G49 all you need is current machine position. In my machines #5043 is current machine position so in my macros I cancel with a line of G49Z#5043. For the G43 I gather my tool offset via parameters. So I set #537=#[2000+#20]+#[2200+#20]. #20=tool number. Now #537 is equal to my tool offset so the G43 line looks like so. G43Z[#5043-#537]H#20(#20=tool number). Basically this always sets G43 whenever a tool is called so I never have to code this into any program possibably making a mistake.

Stevo

[Brian FRF]

A bit more odd ( I think the g43 h1 thing is working right now)
But, I dont seem to be able to get g54 to load. Ive loaded it though MDI, changed the parameter 6219, and put g54 in several places in the program, still the machine is heading way off from where it should be going?

Maybe I need a z position, not zero to cancel out g43. Basically Im wondering if Im cancelling the drill cycle too fast, so the machine is trying to hit r plane, of .100 above z0, but z0 is tool change instead of part zero. All my positions are saying ~.080 positive z, when I have an overtravel error, coming above tool change position?

[maz43]

Many of these controls default to g91 when reset.
Try this-
N1G0G40G52G80G90
T1M6
G54X#Y#S#M3
G43H1Z1.M8
(MACHINING DATA)
G80
G0Z1.0M9
G40G49Z0.M19
M1

If you still over travel canceling the tool try sticking a G52 in before the G49 line.
Your machine may require G52 Z0 to be set at tool change height.
Same applies for G54-59 Z offsets.
I run a Mazak and Tree VMC that share this trait.
Both have Yasnac MX3 controls.
To set tools this way mdi T1M6
Go to offset page, put in handle jog mode, and push the measure button.
Touch tool to gage block and push write and return button.
Repeat process for next tool.

I run a Mazak and Tree VMC that share this trait.
Both have Yasnac MX3 controls.

Could you post some of your code?

[Brian FRF]

Ill post up the programs Ive got written now, and working.

Couple weird things Ive noticed:
m3 and m8 cannot be on the same line, I get a duplicate error
549 and g52 have to be in order, and I believe on separate lines as well
Seems once I finish the tool use, Ive got about 6 lines of canceling things, turning off spindle/coolant/offsets, etc.

hopefully you folks can help me clean up some of this mess!

Interesting, is to get my offset working, after I home the machine, I have remind it if you will, with a g92x0y0z0 at the home position.

Also thanks for the list of program trick (alarm, page up) I found hour use as well. This machine has been on for ~2800 hours, and "feeding" for 560 hours. Sounds low to me, sound low to anyone else?

[beege]

Curious thing about M3, M8. I've never run your Yasnac, but I've run a bunch of others. M3 is spindle forward, yes? and M8 coolant on? M13 used to be "spindle forward coolant on". Have you used that before?

And since you have 6 lines which never change, could you make those 6 lines into a sub-program that you call on just one line?

[stevo1]

Beege,
I have had that function on a few machines I installed, programmed, and ran. It is pretty cool. We had M13 for spindle CW coolant on, and M14 for spindle CCW and coolant on.

Stevo

[Brian FRF]

Ill have to check into m13, never heard of it.

As for the 6 lines, here come programs, so youll see what I mean. With the tool number changing in there I dont hink it would be practical. Frankly I think I have too much junk, that I just dont need. Other programs that were still in the machine dont have this much stuff, and I believe most of the programs work (only tried a couple)

So, programs, as promised!
material is 3/8 x 2 mild steel bar, 7" long. drill is 1/2" and end mill is 1/2" HS right now (rather bust it than a carbide!) Its in soft jaws. End result part is 2 .720 holes, 5" apart, and radius on each end. VERY exciting complicated part!

drill program
O1000
G40 g90 g49 g80 g20
M6 t1
G43 h1 z1.
G54 m3 s800
M8
z.1
g73 x 1. Y-1. R.05 z-.65 q.05 f4.
X6.
G80 m9
M5 z0
G49
G52
G0 z0
M19
T2 m6
M30


end mill program
O2000
M6t2
G17g40g90
G54 m3 s800
G43 h2 z 1. M8
Go x 1. Y -1.
z.1
g1 f10. Z-.4
g12 i.11 d.11 f5.
Go z.1
X6.
G1 f10. Z-.4
G12 I.11d.11 f5.
Go z.1
y-2.27
g1 f10. Z-.38
g3 x6. Y.27 r1.27 f4.
G0z.1
X1.
G1. F10. Z-.38
G3 x1. Y-2.27 r1.27 f4.
Go z.1 m9
M5 z0
G49
G52
Z0 m19
M6 t1
M30

[dcoupar]

Matsuura didn't have M13, and you can only program 1 M code per block. You can, however program multiple G-codes in a block, as long as you only have 1 from a group (no G00 and G01 in the same block). Also, if IIRC, you MUST move Z to home before the M06. So your startup code for each tool should have G00 G49 G52 G90 Z0 to be sure Z is at ATC position.

I would recommend that you strive for consistancy in your programming for easier readabilty and troubleshooting your programs. Try the following program and see if it works for you.

%
O1000
N1 G40 G90 G49 G52 G80 G20 Z0
M6 T1
G54 X1. Y-1. S800 M3
G43 H1 Z1. M8
G73 G99 R.05 Z-.65 Q.05 F4.
X6.
G80 M9
G49 G52 Z0 M19
M1

N2 G40 G90 G49 G52 G80 G20 Z0
M6 T2
G54 X1. Y-1. S800 M3
G43 H2 Z 1. M8
Z.1
G1 Z-.4 F10.
G12 I.11 D.11 F5.
G0 Z.1
X6.
G1 Z-.4 F10.
G12 I.11 D.11 F5.
G0 Z.1
Y-2.27
G1 Z-.38 F10.
G3 X6. Y.27 R1.27 F4.
G0 Z.1
X1.
G1 Z-.38 F10.
G3 X1. Y-2.27 R1.27 F4.
G0 Z.1 M9
G0 G49 G52 Z0 M19
M6 T1
M30
%

[Brian FRF]

Ill try these. Ive got to rewite pretty much anyway, since I want it as a program, and I just got the second vise on, so Im going to usie these as subs, and 2 work coordinate systems in here.

We shall see what happens now!

On a side note, anyone know how to change the settings in this forum so I dont get all these threads upsidedown? (#13 first, and #1 last), just confuses me!

Matsuura didn't have M13, and you can only program 1 M code per block. You can, however program multiple G-codes in a block, as long as you only have 1 from a group (no G00 and G01 in the same block). Also, if IIRC, you MUST move Z to home before the M06. So your startup code for each tool should have G00 G49 G52 G90 Z0 to be sure Z is at ATC position.

I would recommend that you strive for consistancy in your programming for easier readabilty and troubleshooting your programs. Try the following program and see if it works for you.

%
O1000
N1 G40 G90 G49 G52 G80 G20 Z0
M6 T1
G54 X1. Y-1. S800 M3
G43 H1 Z1. M8
G73 G99 R.05 Z-.65 Q.05 F4.
X6.
G80 M9
G49 G52 Z0 M19
M1

N2 G40 G90 G49 G52 G80 G20 Z0
M6 T2
G54 X1. Y-1. S800 M3
G43 H2 Z 1. M8
Z.1
G1 Z-.4 F10.
G12 I.11 D.11 F5.
G0 Z.1
X6.
G1 Z-.4 F10.
G12 I.11 D.11 F5.
G0 Z.1
Y-2.27
G1 Z-.38 F10.
G3 X6. Y.27 R1.27 F4.
G0 Z.1
X1.
G1 Z-.38 F10.
G3 X1. Y-2.27 R1.27 F4.
G0 Z.1 M9
G0 G49 G52 Z0 M19
M6 T1
M30
%

[beege]

On a side note, anyone know how to change the settings in this forum so I dont get all these threads upsidedown? (#13 first, and #1 last), just confuses me!

"User CP" on the top of the page, down to "Settings and Options", "Edit Options", scroll down to "Thread Display Options", "Linear, Newest First".

Play with them, maybe there's an option you'd like better.

[Brian FRF]

got it running nicely now. 2 sub programs, 2 parts. Ill post the program in a couple days, see if there is anything to clean it up, looks pretty good. Thanks for the clean up already!