tool lenght offset in mazak

[Haroon]

Sir,

 

I am an avid reader of your magnificent forums, it’s really a great place to learn from the masters…. thank u everybody in advance.

 

I have a problem with setting up the tool length offset for a Mazak vmc with m32-b mazatrol control, I am using the EIA command page to get G54, 55 and mc 9.1 to generate the tool path. And I am getting the program and the work offset 100%. But I have a problem in getting the tool length offset.??? I am using the same procedure I used on g54, 55…. but the machine keep giving me wrong tool length offset????

 

i changed the g codes in the program from g43 h1 to g44 h1 and I put the tool length offset in + and still I am getting the same wrong values????? this is the only way I know to set up the tool length offset.

 

(this is my first time in front of mazak machine and the boss pushing us hard to use mc9.1 & eia on this machine…) any help please….. and sorry for my bad English

[Jimmy Wakeford from Barefoot CNC]

Is this scenario?:

 

+ H1 offset

G54 Z offset puts Z zero to top of part and H1 holds the positive gage length of tool for G43. (should cause tool to be raised up value of offset.)

 

Or?:

 

- H1 offset

G54 Z offset is at machine Z zero and H1 holds the negative distance The tool moves to touch top of part with G43.(Causes tool to move distance H1 down)

[Jack Mitchell]

haroon,

 

Welcome to the forum.

 

You are going to use the tool length measurement probe on this machine.

You are also going to use the Mazatrol tool length and tool diameter defaults as well.

 

Having Mastercam and using the tool diameter and length functions are as simple as changing two machine parameters.

 

Please do a search within this forum on Mazak or Mazatrol - for these issues have been well covered in the past.

 

Regards, Jack

[Haroon]

thank u sir , i will do my search .

 

regards

[Jack Mitchell]

haroon,

 

As I recall the machine parameters are F91, F92, and F93.

Please only use the standard tool file and Do Not Use the secondary access screen because this will not be necessary.

 

G54 thru G59 will need to be used, all the rest is driven from the Mazatrol tool data screen.

 

 

Regards, Jack

[Haroon]

jack sir ,

 

thank u very much , i will check the machine parameters on monday , hope it will work.

 

regards

[crazy^millman]

Jack is right on the money been a few years now since I had to do this but I would do it this way. I use to write my nc programs complete as sub used by Mazatrol. I however on a VTC-30C PC Fusion 640m used the Mazatrol as my G54 or if I remember correct WCS to postion my parts. I think it really comes down to personal preference and what you feel comfortable with and like using. The G54 fixture offset is a standard format where as the Mazatrol Method is I guess some what off the wall but worked for me.

[Haroon]

Jack Sir,

today i checked the machine parameters

and they were f91 00010010

f92 00101000

f93 00000000

do i have to change anyone of them ????

 

regards

[crazy^millman]

What does each mean in the book for parameter you should see a explation of each hex decinmal code they are read from right to left on a Mazak to change the parameter you need to type the whole 8 number but with the change if i remember correct you may have to type the allow code for changing parameters something like 1311 on page i can't remember. I am sure Jack or someone else know off hand know they have done it.

 

[resjun]

ill check my machine tommorow vtc 200c fusion i did on the mazak at work so much better

[Jack Mitchell]

haroon,

 

Here they are - but do not use them if your supervisor is unaware or if you do not have the operation manuals with a proper explanation of each parameters function.

 

Still want to change them?

 

Make changes then power down control.

Power back up.

Run a fake G54 so as not to crash.

Use an initial level of 2.00", single block, control reset, then check each tool with a 123 block.

 

If your machine has the MP10 or MP12 Renishaw tool measurement probe, the macros will auto measure diameters & lengths.

 

If your machine has the mazak plunger style then auto measure will do the lengths only - you will have to mic the diameters and input these values.

 

All Eia information will be gathered from the Mazatrol Tool Data information screen automatically.

 

F91 00010000

F92 10100000

F93 00001000

F94 11010100

F95 01000101

 

I realize that calling people sir is sometimes cultural or meant as a form of respect; Please just call us by our names, as we also do for you.

 

 

Regards, Jack

[Guest CNC Apps Guy 1]

We use negative values in the G54 etc... offset in Z and have positive numbers (Gage Length) in the tool offset. The reasoning behind this is that we touch off tools on a common point that never changes then if a tool breaks, I'm not dependant on a surface that may or may not be there anymore having to constantly adjust to bring something in.

 

JM2C

 

[Haroon]

jack

thank u very much , i will have my supervisor with me when i will change the parameters

 

( resjun , james , millman thanks ) i really appreciate your help friends.

 

 

regards

[crazy^millman]

Yeah Jack came through on that one. Good Going Jack.

[Jack Mitchell]

Actually, the Renishaw Mp10 & Mp12 are the contact probes for setting part zero.

 

I cannot recall the name on the Mazak/Renishaw tool measurement unit - something like Sr25 - cannot remember.

 

 

Regards, Jack

[SLJ]

Place I used to work had about 20 mazak mills. All the way from M1's to fusion640's. It's been too long now, but as I remember it, we had them set up to take dia. from the mazatrol page, and length from eia. Put in dia. comp as diff. from tool standard(wear comp). Had to have the param. set to split the recommended setting. Mazak service people argued it would never work out, but we ran all of them that way for as long as I was there and several years before. Wish I could remember more details for you. Steve

[Jack Mitchell]

Steve,

 

I run my machine (M32) off the secondary page using offset 1 thru 16 as tool length comp and offset 17 thru 32 as tool radius comp for years on end.

 

The method described takes all info from the Mazatrol tool data screen and works very well.

I personally never worked the M1 control, but I have probably worked the rest of them cept for the integrex and variaxis.

 

 

Regards, Jack