haas vf5 tool lengh offset

[ChrisH]

Ok I have never run a haas but have run many different mills with a tool changer. (hurco-mazak-ingersoll-toshiba-viper) On all of them I set all my tools on a common spot like top of table and used an offset for each job so I don't have to set each tool over and over again for each job. The machinist running the haass that I program for says that you can't do this on the haas vf5 that we bought 6 mounths ago!!!! Can anyone back me up and let me know if this can be done on a vf5. I have looked thru the book and I can't see the problem with setting all the tools on the table.

 

 

Thanks for all the info!!

[Trevor Bailey]

Of course you can. What is his reasoning? The HAAS control is still basically a Fanuc style.

 

Is it a 5ax?

[jkilby]

We set them off the bed and us offsets. We have a VF-1 & VF-6

[Eric S.]

I do it all the time on our VF3 ANd VF2 Mills.

 

That is the only way to go in my book.

[Jeff2005]

You can but it would get confusing for anyone else running the machine other than just one person.

 

We just had this discussion at work, we use a probe to set our work and the tool setting device, our probe quit working and this topic came up, on how you would set your tools from the table. It was a good discussion I still don't totally understand it myself but I know you can set it from the table, but like I said it would be dangerous to do so if you have different people running the machine.

 

question: How are you setting the tools now?

[ChrisH]

my forman is listing to them and telling me that it does not work like that. And it can;t be done! I'm going to have to work late after they go home and set it up for myself and show the forman. I read over the book and give it a shot.

 

Any suggestions are welcome

[Eric S.]

Dangerous??

 

Your table does not change height?

Set a standard. ALL TOOLS SET ON TABLE.

 

Done

 

Why would you want to keep re-setting you tools? each time you change jobs?

[ChrisH]

quote:

---

question: How are you setting the tools now?

---

they set each tool for each job depending on were the Z0 is. Changeing each toolengh for every job that has a different Z0.

[Eric S.]

Try setting up more than 1 job up at once that use the same tools and see which works better.

[Jeremy Grigsby Excelsior Marking]

This is told to you by someone that has never done it that way. We have a vf1 and I would think all the vf series are the same basic principal. We use a electronic plunger type toolsetter. It's got a set height, and you just bring all the tools down to touch it until the light comes on indicating contact. Then we use an electronic edgefinder to set the xyz offsets of the part. The electronic edgefinder also has its offset set with the plunger. When you find the top of the part with the edgefinder, you hit part work offset button while on Z, G54 G55, etc... Then you go to the offset page and find the tool offset for the edge finder. Type the tools offset into the input field as a positive number. Before you hit enter, go back to highlight the g54 z offset, and press enter. It will add the lenght of the edgefinder and all the tools will be set to the top of the part. The plunger thing is more accurate than paper, plus you don't chip your tools accidentaly.

[Eric S.]

Chris you set the z work offset for each job.

eg.

tools set from table.

Z value work offset is is the height of the programed z zero.

[mmphoenix]

Sure you can do that. Go to setting 64 (T. OFS MEAS USES WORK) and change it to ON. Then get you a master tool that will never change in length (we use a 3 axis electronic edge finder in a holder that we fixed so it wouldn't move) you will use this tool to touch off on the part or table or where ever you want. The thing to remember is when you want to set the off-set for that master tool instead of hitting the tool off-set measure button you need to hit the part zero set button. Then if you know your tool length off-set on your tools you just have to type it in the control in the correct tool location. Basically what your typing in the control is the length difference between the master tool and the tool used to do the machining. You do have to have the positive or negative sign entered in the control when typing in the off-sets. We use a pre-setter on all of our tools, so we know the tool length off-set when we set up on a job. Then all we have to do is touch off with the master tool and type in our length off-sets in the control and we are ready to go. You should find some info in the machine manual but if not then call your Haas HFO and talk to a technician and they can help you out.

[ChrisH]

thank that sounds like the way to go. I'm a little lost but it will come to me when I get some time on the haas controler. Like I said I have never ran a haas. I'll see If I can get some time to mess around with it next week!

 

Thanks mmphoenix

[Jeremy Grigsby Excelsior Marking]

Mmpheonix and I have the same post but worded different

[Chris Rizzo]

All our Haas' are set up like what your after, Chris. Pretty low-tech, with no probes or such, but easily accurate to the tenth'.

 

-Settting 64 is set to OFF.

 

-Tools are all set to the table. I use a .500 dowl pin as a go / no-go gage. Press tool offset measure. Enter -.500, to account for the dowl pin.

 

All tool length offsets are thusr minus values -.

 

G54 Z0. is set as height "up" off of the table. Plop a height indicator on table, and enter value into g54 z offset.

 

All work offsets are positive values.

 

You now can run any program you want, and never have to change a tool offset value. Only thing that you change is g54 z.

 

hth.

[ChrisH]

thanks Mmpheonix and jeremyG they are both lots of help. The more input the better

[Chris Rizzo]

quote:

---

my forman is listing to them and telling me that it does not work like that. And it can;t be done!

---

Challange your "[on]crack team" of machinists and foreman to a race. Change set-ups on a machine between two programs, each running 10 of the same tools. See who's ways faster, your's or their's.

 

You'll have to change g54 values, they will have to change g54 AND H 1-10.

[ChrisH]

Now do the right z values show up on you position page when activate g54 and the h value for the tool your using? I ran a Mazak the z value was not right on the position page when you ran dnc with tool offset on. It cut fine but the z showed a different number. If I ran something that I programmed in the controller it showed the right value.

 

I hope this make sense

[ChrisH]

stylin

 

Do ever use the live spindle were you can move the z up or down during a program to help blend. I was told that it does not work well. He said it will crash about 50% of the time.

One more thing is there a good way to lift your z and change an insert and start back were you left off. I was told that you have to edit the program and restart it a few line back. Most of the mills I have run you could press a button and raise z and change the insert then just press cycle start and It would feed back down and take off cutting. The machinist wanted me I put a retract after every pass so he can change the insert. That is a wast of time to cut all that air.

[MATT Q]

Sounds like those guys are messing with you. That doesn't sound very productive at all.

[crazy^millman]

You will miss the Mazak for ti ability to changes tools on the fly. HAAS does not have this option. Fadal does but not HAAS.

 

Sorry for the Bad news.

[ChrisH]

I have not had any input in this department till now. I’m trying to change things for the better. Thing are not GOOD at all. Lots of bad habits pasted on for one to another. If some one new comes in they would tell the new guy this is the way we do it.... I think that I can get things done with this forum backing me up. I was told that (it’s not that bad)

 

My Forman read all your comments and he sees the light.

[ChrisH]

ron

I loved running My Mazak. One of the best bridge mills I have ever run.

[Chris Rizzo]

quote:

---

Do ever use the live spindle were you can move the z up or down during a program to help blend. I was told that it does not work well. He said it will crash about 50% of the time.

---

Not sure what "live spindle" means...what does he mean by "crash", software or hardware?

 

If I'm not getting a proper blend, I can almost be guarenteed it's a g54 work offset, and not a tool offset. I will add a few thou. (+.00XX) to g54 z to leave more material, subtract (-.00XX) to take more off. All the while leaving my tools alone. Obviously it won't adjust until another g54 at a tool change or whatever.

 

Like I said before, setting tools with a GOOD dowl pin and off the table it's not hard to get .0001 accuracy, (well, more like CONSISTENCY) on H values.

 

If Mr. Operator want's to look at each insert every few cuts, there are a bunch of diff. options. Null tool change, etc.

[Jeff2005]

CHRIS IF YOUR RUNNING A NEWER MODEL HAAS THEN YOU CAN START FROM ABOUT WHERE YOU LEFT OFF DEPENDING ON HOW FAR AHEAD YOUR MACHINE READS WE ALWAYS BACK IT UP ABOUT 500 LINES AND THEN DO A RESTART. OUR MACHINE WILL READ THE CODES THEN START WHERE YOU HIGHLIGHT THE CODE. I RUN AND PROGRAM A VF-5 3 AXIS.