Haas VF fixture offset hell

Hi Byte,

Comments/suggestions are below....

Can't help you with the particulars of the HAAS control, but if I understand you correctly, your question is : "How can I avoid having to pick up the tool lengths every time I change setups (or even change the Z position of a job)?"

This is pretty easy, and it makes alot of sense IMHO....make your tool length offset value equal to the distance from the programmed point of the tool (almost always the very tip of the tool) up to the spindle nose (a ~small, positive Z value). When you set your Z work offset, this value should be the distance from the spindle nose down to the Z0.0 point of your part (a large, negative Z value). Any time you change the Z0.0 position of your job, you will have to pickup your Z work offset, but your tools will still be OK from job to job/setup to setup....

And please don't suggest I use a different H for

With the above method, this is what happens....

Holler if you've got questions.............Brian

I can't tell you what is correct, but this is how I do it.

I set all my tlo's on the table (or 1x2x3 block, or whatever as long as it stays the same).

Then, I put my indicator in the spindle, and touch it off on the table, zero the relative, and touch it off on the top of my part. The number on the screen goes into the z position of G54 (or whichever you're using).

Dave, I have 3 of those machines, I do the following: Set all of the tlo's at 6" above the table, (2 1-2-3 blocks stacked), this does 2 things.

1) it is very easy to grab 2 blocks and get going. 2) My 6" pocket scale is a quick reference for what follows.

After all tools are set, I go to the "top of the part", or whever program "z" zero is going to be, and dial the last tool set to that point, using a .250 pin, I roll the pin under the tool moving .001 per click UPWARD, until the pin goes under, then I move off the part and dial down .250.

(Part accuracy dictates whether you go .001 or .0001)

Then I calc the difference between the machine position and the tool offset value for that tool and this gives me the value to put in the work coordinate z offset, if it is not obvious as to whether it is positive,(taller than the 6" tool set height) or negative, (opposite), I will then throw the scale next to the part to double check.

I can use any tool in the turret now for any job, as long as I do the work offset setting step

This sounds like a lot of work, but it has saved my a$$ more than once!!

As far as the returning to default #'s, there is a setting in the machine that will reset all defaults at "reset".

Hope this helps. Darrell

Dave Ly> >

Yes. What I meat is once you put a tool in a mill you should only have to set it's tool length offset once. From then on, you only adjust the Z values of your fixture offsets.

Are you doing this offline with a height gauge? I'm familiar with that method. I ran a Fanuc/Makino were we set tools that way.

My gripe is, I think you should be able to do that using only the tools in the mill.

Nice method, I'll have to try the pin sometime. You could probably eliminate chipping delicate tools with it, huh. I've been using .001 shim stock forever.

When you say 'calc the diff' are you actually using a calculator?

That's my goal.

See that's what's killing me, I have to make sure there is no active Z fixture offset other than 0.0 or it won't work. AFAIK

I just think I should be able to do this without the use of a calculator, a height gage, an indicator, 6 Our Fathers, 3 Hail Mary's etc.

Hi Byte,

Comments are inline below....

This is possible without any special/dedicated measuring or calculating equipment....you simply use the machine as it's own tool presetter....

1.) Remove the tool from the spindle.... 2.) Touch the spindle nose on the top of something clean/smooth/flat...how 'bout a 1-2-3 block? 3.) "Zero" your position screen...(use your position display page like you would a DRO on a knee mill). 4.) Place the tool you want to measure back in the spindle, and now repeat step #2 (being careful to not damage the tool...doh!). 5.) Make note of what your position page reads...this value is what you want to put in the appropriate tool length offset register. (Various controls have ways to input this value automatically to minimize the chance that you'll mis-key the value). For a quickie sanity check, get your 6" scale and visually check this (the distance from the tip of the tool to the spindle nose). 6.) When you go to pickup your G54/G55/etc. (or whatever your control wants to see to assign a program zero position), be sure to measure from the same surface on the spindle nose to the zero point of your part. This number will represent the distance from the spindle nose to the zero point of the part when the machine is at Z home (this will be the value you want to input to your work offset's Z register).

I may be wrong here, but I think your difficulties might have more to do with not understanding what the control is actually *doing* when it uses different types of compensation (in this case, the use of tool length compensation and fixture offsets together), and less to do with what G-codes to use or keys to push to get it to spit out good parts.

Cheers...............Brian

Byte, yup, I do use a calculator, takes about 10 secs to do the math, have used this method on very simple vise set-ups, to complex 4th ax. rotary set-ups, very few, if any mismatches, and, as long as the programmer (me) hasn't botched the program, things run well.

Are you using the set tool offset - next tool buttons?

FWIW, I run mostly 1-5 pc work, much of it expensive stainless and quite a large amount of racing engine blocks that you wont get a second chance to f up.

Not braggin, just have a method that works well and produces "one shot, one kill" type of results.

BTW I can set 25 tools and pick the work "Z" on my vf-5 in about 10 mins. using this method.

Darrell

That's the way I do it on my haas, except I use my edge finder (the light up kind) to set the Z. But what do I know I'm a lathe man.

So you move your Z slide to home, then zero like step 3 above, before you touch off part zero? That would get rid of the problem I have with needing a fixture offset with a Z0.0 active before I touched off. I found out a while ago that when I hit reset, G49 becomes active, which cancels any length offset. Now if I can figure out how to cancel the fixture offset when I hit reset I can use the method In my first post.

That's why I'm posting. Just trying to grok the problem so I can make an informed descision on the easiest and most bulletproof way of doing this.

Yes, when I first install tools into the mill... wheel the tool down tool offset measure next tool rinse and repeat

That is elegant!

I've been wanting to try one of those for a while. I have a tool setter on my Mazak though so I'd have to figure out a way to teach the 3 axis edge finder, with both the tool setter and the edge finder being spring loaded. Come in handy for checking relative heights of surfaces too, huh.

I do the same thing with the .250 pin and it does work great. Feeding UP to fit the pin under the cutter really saves those brittle carbide cutter tips. One thing I have to do to get the proper depth is figure the z backlash. On the machines I set up I have to add a couple .001's to the pin diameter to get to the same depth when feeding down. On 1 machine I have to figure .002 and another .004 then when I take a cut the depth is just about right on. Maybe time for some calibration work. Duffy

My edge finder is not spring loaded. All tools are set off the table on a 2" block. New job bring edge finder down to 2" block, press origin , move up to top of stock, bring down to top & enter the numbers shown into the G54 or whatever offset you use in the Z . Works on my hass. One setting for a new job "If" I can use the tools already in, if not only set the new tools off the 2" block on the table. Say it's just like the work shift I use on all my cnc lathes, I just tell the control where the bar is in Z & all tools in the turret don't need to touch off any tools that have not been changed.

I have seen people on mills touch off every damn tool on a new job even tools that have been there. But what do I know I'm a lathe man. I'm lazy... Why touch off a tool that the control knows where it is?

All I know about mills is the table is always in the same place.

What flavor edge finder do you use? I've never used one of those 3 axis type. I just assumed the Z has some kind of spring in it.

That's how you guys are getting around my problem of having to make sure the active fixture offset has a value of 0.0 in the Z coordinate. You're zeroing out your display, like Brian mentioned. Cool.

You think that's bad, I've seen people put a different H for each tool at each fixture offset just to keep the Z coordinate of each fixture offset at 0.0. Different H's for the same tool has its use, but not in place of fixture offsets.

It's Friday with 10 minutes to go. 6:30PM to 3:00PM hours are great. Although I'd rather work 4 tens.

Get a 123 block, take tool out of spindle. Decide where Z 0 is. Crank spindle face down to roughly 2.9 above Z 0. Start moving Z up until 123 block just slides under spindle face. Goto work offset page choose appropiate work offset, highlight the Z field. On our Haas VF-3 there is a button in the upper left area that has printed on it "Zero set". Type a 3. and push Zero set this will set the Z 0 to the proper height. Go to MDI type G90 G53 Z1.5, this will send the machine home. While still in MDI call up the work offset. Put tool in spindle and repeat the Z touch-off procedure only use the end of the tool instead of the Spindle face. After finding the tool height go to the tool offset page highlight the Z field on the proper tool offset and push Zero Set. At home right now so some of the syntax might be incorrect but this should get you started. Good luck.

bytecolor:

I have a 3 axis LED edge finder, and it's spring loaded in all directions, Z included. Similar to about the 14th tool down at the following site.

I'm sorry if I'm repeating something someone else said, but I'm having posting/access problems (in fact I don't know if this will even post - but I'll give it a shot). In our Haas VF6 mill, if you hit the "Position" button, then hit "Page Down", you should be at the "Operator" page. Any, or all, of the three axes can be zero'd out anytime you want by hitting the "Origin" button. Another point, the zeroing of any axis on the operator page is independent of any other axis setting on the machine, (read doesn't effect G54-59 or TLO's).

Hell, thats not weird. Here is weird. I took over running a Fadal from a guy who had been fired just as he starting to machine a large casting. He had cut a slot in the top of the casting, apparently by manually moving the axis with the jog wheel. I asked the guy on the machine next to him what the heck that was for. He said that was the finished surface, and now you just set all your tools to that surface! I was new to CNC, but I nearly fell down laughing at that one!

Gary H. Lucas