Tool Data

Has any one found a way to load a partial tool data in a Matrix e-machine. Reason being if we are loading a tool package that just replaces tools 101 - 120, I don't want to have to fat fingure 20 tools in everytime a tool package is changed. I know Cyber Tool is an option but was wondering if there is another way. Thanks for the help.

Well you could text edit the TOOLDATA file (just a thought)

That is you save it via DATAIO (as a text file!!!); Delete/Copy/Paste what you need and load it up into the control via DATAIO again;

*Although I have never done it!* I don't see a reason why it shouldn't work;

I would only make sure that you DON'T change anything!!!

I'm curious if there is some more comfortable way

That's an interesting idea fooo, I gave that a try today and it worked. It seems that each data field in the Tool Data has an address (as below) and is populated when read into the Data I/O somehow. Below is a sample. There are three lines of code for each tool description. So on the first line I changed the D0.39 to a D0.38 and read the file back into the control and it changed my Chamfer NOM to 0.38. Now I just have to figure out what the rest of it means?? Thanks for the idea!

G10L40M0T120P0C13&C0D0.39S0I0H8.64514K0.J0Q28&J0&Q0N01000001W00000000&F0
G10L41M0T120Q0P0K0S0R0E0N0
G10L42M0T120X0.Y0.Z0.&X0.&Y0.&Z0.A0.B0.C0.D0.E0.F0.I0.J0.

Well check your Mazatrol manual.

In the very back there's something called `Three Digit G-Code Format'. There you should find the format of a TOOL-DATA file explained.

BUT unfortunately my documentation is outdated -- that is it doesn't match the file format what I get when I dump a file via DATAIO. In particular the addresses do not match.

Here is a hypothetical example: the book says address E is the actual cutter dia but in the file it's encoded with a D.

However the basic structure seems to be the same and it should give you some idea how the format works.

Well I'd be very careful to change any values you do not exactly know what it is. I assume copy/delete/paste complete sets between files should be rather safe.

The three lines you posted here form a complete tool set (as far as I can tell). L40, L41 & L42 represent a logical unit together.

When you actually CHANGE values you should pay attention to the data types used for values (numbers). To me it looks like there are three types in use: integers (numbers WITHOUT a decimal point); floats (numbers with a decimal point) and (8)bit fields (like N01000001 in your posted example). As an advice I'd make sure not to change the type of a value!

Well if you have documentation which is up-to-date let me know as I have been looking for this.

I think three digit G code format for mazatrol tool data will allow you to append only one tool, if that's all the info you are sending in. In contrast to mazatrol file format, where you must overwrite the entire contents of tool data.

if you switch to text output and output the tool data file, you can pick out any one tool data and glean what the text means better, but you guys already know that.

back up your pristine tool data, and do some experiments.

jim

@Tobor
Have you checked your documentation yet? Does it match the file format?

Would really like to know;

Hey sorry guys, was on vacation. I looked in the back of the Mazatrol manual and sure enough there was the 3 digit explanations. It looks to be correct so far for the first tool. I have to go through the rest. I have the Matrix manual for Integrex e machines. I'll let you know what I find. Thanks for the help!

@Tobar

Can you check something for me?

In my manual at the very beginning of the chapter "Three Digit G-Format of MAZATROL Program" it shows the header of such a file; There's a version number field (or something like that); In my book it says MG3-251 -- what does your book say?

The files on our machine have version MG3-252;

The manual I have is H740PA0054E and the code MG3-252...
Maybe and updated version?

Cool! Now I know at least what I have to look for;

Any chance somebody has this handbook as PDF and can send it to me?

Ok got it thanks a lot!!!

I can send you the H740PA0054E manual... coming right up.

This was given to my by a Mazak Service fellow who shall remain nameless.

I have used it for a few of the options, but never for all of them so I cannot guaruntee its accuracy.

With this, you can create a file with all your tools 1 - whatever (if you wanted) and store all the data in said file, if someone does something dumb, you just throw the file in the machine, hit Cycle Start and you have everything back....Assuming they all work.

If someone has the time that I dont have to try it all, that would be sweet.

#3022=120.01
#700001=#3023 ( TOOL INDEX NUMBER )
#701001=18 ( TOOL GROUP TABLE *1 )
#702001=#620 ( LENGTH A )
#702002=0 ( NOSE-R / ACT-DIA)
#702003=0 ( 0= LIFE OVER OFF 1= LIFE OVER ON )
#702004=0 ( 0= NO BROKEN 1= BROKEN )
#702005=0. ( WEAR COMP X )
#702006=0. ( WEAR COMP Y )
#702007=0. ( WEAR COMP Z )
#702009=-7.387 ( LENGTH B )
#702010=0 ( 0: NO INSTRUCTION 1: INSTRUCTION)
#702011=2. ( 1 OUT 2 IN 3 EDG 4 IN BAK 5 EDG BAK)
#702013=.1968 ( NOM DIA. )
#702014=0 ( 0 NORMAL 1 MG+ 2 MG- 3 LARGE 4 SMALL)
#702015=1 ( 1 TO 26 A TO Z)
#702016=0 ( ID CODE ATTRIBUTE 1= HEAVY ATTRIBUTE )
#702017=0. ( INDEX ANGLE 0 TO 359.9 OR FLASH TOOL )
#702018=3 ( CUT DIR 1= RIGHT, 2= RIGHT, 3= LEFT, 4= LEFT, 5,6)
#702019=0 ( CUT ANGLE 0 TO 999.9999 )
#702022=0 ( EDG-ANG 0 TO 999.9999 )
#702024=0 ( WIDTH 0 TO 84.5 )
#702026=0 ( 0 TO 4 NO HOLDER TO HOLDER NO 4)
#702027=2 ( 0 TO 2 0 STANDARD HOLDER)
#702028=0 ( LIFE TIME 0 TO 9999 )
#702029=0 ( CUT TIME 0 TO 9999 )
#702030=0 ( LIFE NUM. 0 TO 9999 )
#702031=0 ( USED NUM. 0 TO 9999 )
#702034=.1968 ( ACT DIA CO. *3 TABLE 0 TO 84.5 )
#702035=0 ( ACT DIA CO. NO/ OFFSET NO *3 TABLE 0 TO 2000 )
#702038=0. ( MAX WEAR X 0 TO 9.99)
#702039=0. ( MAX WEAR Y 0 TO 9.99)
#702040=0. ( MAX WEAR Z 0 TO 9.99)
#702041=0. ( EASY COMP X -9.9999 TO 9.9999)
#702042=0. ( EASY COMP Y -9.9999 TO 9.9999)
#702043=0. ( EASY COMP Z -9.9999 TO 9.9999)
#702044=0. ( CONS.COMP X -9.9999 TO 9.9999)
#702045=0. ( CONS.COMP Y -9.9999 TO 9.9999)
#702046=0. ( CONS.COMP Z -9.9999 TO 9.9999)
#702047=0. ( LENG COMP. -84.5 TO 84.5)

Thanks Milling Man!

I could not find a system variable for the ID code (A,B,...), talked to some good e machine apps guys in KY too.

Will try and let everyone know.

The G10 (from earlier) is an I/O format so it's not programmable (some do work but it's incidental).

The format Milling Man posted will write any tool data on Matrix for mill or lathe tools and is completely adjustable "on the fly" in a program. The key lines here are:

#3022=120.01
#700001=#3023 ( TOOL INDEX NUMBER )


In the above, the "Tool Index Number" is NOT the prefix used (like A, C, heavy G, etc). #3022 is only where the prefix is picked up. #3023 is an index number that the control assigns and tracts when using mulitple prefixes (in case the manual is confusing about this). For example, if T34 is only created, index number is generally 34. However, if you have T34A and T34D, an index number is assigned.

I have used all of them and they all work. You can use any of them as well. It's only effective one tool at a time so for addtional tools, you need to reflash the first 2 lines again (otherwise you just end up writing over the same data).

I'd have to check each variable listed one by one but it looks like you got it all there Milling Man

BTW.... your Main A/B version needs to be at least B5A for this....