yasnac mx1 on matsuura programming help needed

[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]

Originally Posted by 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.

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?