help with haas offsetts

[cherokeechief79]

ive used a lot of haas mills is several different shops and all were set up the same way.today i finally got to run one of the haas mills in the new shop im working in.i was happy because i knew that this will finally be an easy task for ne after nearly 3 weeks of learning new machines and controllers.(ive been on a conversational hurco for a week)i wrote my program fine and set my offsetts as i always did.i edgefound the upper y and set the y g54 then i put -.100 and hit write.i did the same for my x which had a stop on the right side.instead of subtracting .100 from each side it added .100 and the holes were way off.i did it again and this time i put -.100 in the x and y g52 box.the same result.also i tried to run the program 5 inches above the part by putting 5. in g52 z but the tools wanted to go 5 inches deeper than programmed .
im sure this is one of the settings that is doing this but is this the way most of you program?

[Delw]

are you sure your program is running the same fixture offset and the same tool length number that you set? ABSOLUETLY SURE?

Ive done it as few times thats why I mentioned it.

[Geof]

Haas has three coordinate system modes in which can operate, Haas, Fanuc and Yasnac and these change the way G52 operates. The mode your machine is set for will be Setting 33; go the the Settings page type 33 and press the down arrow to find it.

It is likely your machine is set for Haas or Fanuc, I always use Fanuc so my desciption here is based on that. In either Haas or Fanuc G52 is not a work zero like G54, 55 etc; in these modes G52 is to to set a local work coordinate so you do not enter anything into the G52 table by hand.

The way you describe for G54 Y sounds correct; touch off at the back with the edge finder and press ZERO PART SET, then type in the radius of the finder which is your -0.1 and press WRITE. Same procedure for X and if you are touching on the right hand end you type -0.1 but for the left side it is 0.1.
But I just remembered something: PARAMETER 57 has item 25 NEG WORK OFS and if this is a zero it changes the way the offsets are entered; I always have it as a 1 so if yours is 0 my description is going to be backwards I think.

For moving everything up 5 inches for a safe run the only ways I know are to put 5.0 in the Z column for the work zero you are using or have a G52 command at the start of the program that reads G52 X0. Y0. Z5.0. This moves the Z work coordinate up 5 inches and to run the program correctly you simply change the Z5.0 to Z0.0

[Delw]

doh g52 not g54 etc. make sence to me now.

Geoff what book do I find all those parameters/settings in?

[cherokeechief79]

thanks....ill look at what it is monday.
i have always used g 52 to fine tune ALL of the other offsetts.g54-55-56 etc.if they all had to be moved up .005 i would put .005 in the y g52 value.same with the x or z.iff all of my offsetts were off the same mount i could do this if they were off differnt amounts i would have to adress them seperately in the z value for eack offsett

[Geof]

doh g52 not g54 etc. make sence to me now.

Geoff what book do I find all those parameters/settings in?

The Haas VF-SERIES PROGRAMMING AND OPERATION MANUAL dated JANUARY 2001 that is on the shelf just to the left of my monitor.

Maybe I am being too much of a smart ass.

Back then the manual ran to over 470 pages and had all sorts of stuff about Settings, Parameters, Alarms, etc which seem to be omitted from the manuals these days.

I am sending you a PM.

[Delw]

Your not being a smart ass LOl they pretty much dumbed down all the manuals anymore, I have fadal manuals laying around from 91 I think the machine came with 5 of them, every little detail, even cad cam systems now do have all the info and you dont get a book, you get a "F1" key on your computer.

for everythign I have I went and got all the PDF files ( sometimes you have to call the manufacturer) and had them printed off. its expensive but there is nothing like a paper manual sitting in front of you when your trying to figure something out. not to mention its faster than useing a PDF file online or on your pc, witht he exception of having a extra monitor tapped into your pc then one can be the programming software and the other be the pdf file.

tried taking a laptop out to the machines but every time I do it gets dropped, coolant spilt on it or I cant find what I am looking for.


Thanks again.
Delw

[cherokeechief79]

i looked at setting 33 today and it was set to yasnac.there are 3 options haas yasnac fanuc.i changed it to haas and the x y offset now moved in the direction i wanted it too but the z still moved down more with a positive number.i guess ill just have to get used to this.the way i used to use g52 was great because i knew exactly where xyx zero was.most of our 1st ops were centered in raw stock so i would just add say .032 to y and x in the g52.op 2 was usually exactly to the xy corner so i woud just take the value out of g52.this was way easier than adding .032 to the g54 y and x especially when running multiple parts.my true x and y zero was always the same number.
another thing i cant get use to here is that they take a 4 inch gage block and touch off the spindle nose to the work face for each g54,55 etc.they subtract the 4 inch so that the g54 (or whatever other offset)is now set so the spindle face is now set to the work surface.
i have never done this and it just seems to me that there are now 2 things that have to be touched off instead of one.
i would touch all of my tools off in a common spot wether it be the fixture face,vice top or table.then in my g54 55 56 etc i would put the value from that surface to the top of the part.if i broke a tool i could rest it by touching off of the same location.
do any of you use this method?

[Geof]

.... but the z still moved down more with a positive number....

Did you look at Parameter 57, try changing the NEG WORK OFS and see if that helps.

[cherokeechief79]

thanks!!!!
parameter 57 did the trick

all working good for me now.

on the fanuc setting does the value on g52 actually work?or does it just go away after it reads the g54?
i want to keep it on haas but i will have to make sure the g52 is always cleared out because others here do not use it.

[Geof]

.....on the fanuc setting does the value on g52 actually work?or does it just go away after it reads the g54?....

When the machine is in Fanuc mode any G52 value is canceled by RESET and by M30.

You can also have a G52 X0. Y0. Z0. at the end of your program just to be double sure.