Entering Tool Offsets in Mill

[Geof]

This doesn't have to apply only to Haas but that is what we use so the description is written for a Haas control.

There have occasionally been questions about setting tool offsets. Here is the technique we use with a Toolsetter; it is slightly different to what I have seen described and I think it has some advantages.

The first picture shows the tool being brought down to the Toolsetter until the dial is zero; a close-up of the dial is inset. The Z coordinate for this tool position is entered using TOOL OFSET MESUR. A very important thing to note here is that the top of the Toolsetter must be above the location on the part that is Z zero and must be below the toolchange position. But the exact height does not need to be known.

Offsets are entered for all the tools this way.

The second picture shows a cap with a hole placed on the Toolsetter, this cap brings the dial to zero, a dial gauge is in the spindle and the Z axis is brought down until the spindle dial is at zero. The Z coordinate for this position is recorded and called Zs.

The third picture shows the dial in the spindle moved over to the part with the Z axis brought down until the dial reads zero. In this example Z zero for the part is at the finished surface so a previously machined part is in the fixture. The Z coordinate for this position is recorded and called Zw.

Now the difference between Zs and Zw is obtained; when the Toolsetter has been placed so it is higher than the part Z zero, this difference will be a negative value and is called Zd. Zd must be a negative value for error prevention.

The Zd value is entered into the Z column for the Work Zero(es).

Advantages:

It is quick and accurate. The accuracy depends on the machine and dial gauge accuracy; provided the neither Toolsetter nor the cap are not sitting on a film of coolant which can introduce an error of 1 to 2 thou.

Using a Toolsetter has the inherent advantage that the tools are being brought down to a spring loaded plunger not against a solid block. If the operator overshoots a few thou nothing serious happens. Although if the operator puts the Toolsetter above the toolchange position and hits NEXT TOOL rather serious things happen.

When multiple parts are held in fixtures that have been whipped up quickly and are not as precise as they could be, it is an easy operation to get Zw for each part position and have a specific Zd for each part work zero thus compensating for the fixture error.

When the Toolsetter is at the correct height and the Zd is a negative value it is difficult to get a wrong tool offset. The most likely error, at least in my experience, when entering values is putting in the wrong sign. When the value should be negative and a positive is entered all that happens is the tool goes well above the part and cuts air.

[dertsap]

Originally Posted by Geof Using a Toolsetter has the inherent advantage that the tools are being brought down to a spring loaded plunger not against a solid block. .

my presetter is a 1/2" dowel pin , i always bring the tool below the pin then raise the z until the pin moves below the tool ,
hard lessons learned , i've chipped a few endmill tips in the past

[Shotout]

Have any of you tried any of the elctronic tool setters? I bought one of the cyclinder type, spring load plunger LED lights up when contact is made, .0002 repeatability. I checked it with a height gauge and found it to be 2.0001in. I use that value plus the difference between the tool reference and the part for the appropriate G5n Z value. It has really helped my accuracy but wanted to know what other people's experiances have been with them.

[big_mak]

I bought the probing option with my Haas, it has the tool setter with it, and it's great. Put all your tools in and have the machine set the lengths while you do something else in the mean time.
Best option I bought with mine machine.

[HuFlungDung]

I wish I'd seen the probing thing in action. My noob question would be "How does the machine know when it is anywhere close to where you wish to touch off of, and how does it know which direction to move, etc." I can imagine this taking place in 'slo-mo' but it can't be all that slow or you guys would be complaining about it

[big_mak]

It's not running in rapid, that's for sure, but it does 2 or three probes each at decreasing speeds, so that the accuracy gets better with each trigger.

Maybe if you are nice, I can make a vid and post in somewheres. It will also probe r-comp values as well if you use them.

I've used the work setting probe to size bores. This would update the d-comp register by the radial error so that the interpolated bores would stay on size.

Some trick macro work, but niiice!

[Geof]

Originally Posted by big_mak It's not running in rapid, that's for sure, but it does 2 or three probes each at decreasing speeds, so that the accuracy gets better with each trigger......

So how long does it take to enter the offsets for 10 tools?

[stang5197]

I bought the probing option with my Haas, it has the tool setter with it, and it's great. Put all your tools in and have the machine set the lengths while you do something else in the mean time. Best option I bought with mine machine.

What year is your machine? The machine we bought about a year ago (used '01) has the tool setter but the tech the set up the machine couldn't figure out how it worked. So it has been sitting ever since.

[pit202]

I use fast the same methot as Geof, but I have one constant place for my touch probe so I created a program that come over my "dial" in XY axes, I get Z down with JOG and just press "T.OFS.MESSUR". I have configured it with my 3D taster what I use to get the XYZ for the stock. Hope somebody know what I meant :-) if somebody is qurious how to do it , I can take some photos and describe it more ( or less with my english ;p )

PS.
oryginall probes for haas are too expensive for me , so I try to do my own , with the electronic and connection are no problems, i get only little problems with "time" :-(

[big_mak]

Only takes a couple of minutes. There are options for setting. You can set tools in sequential order, or random order. Then you can check facemills, with the spindle rotating in reverse so that it accounts for any inserts hanging low!

I also use it for tool breakage detection too. This way if you've got your back turned to the machine, it will stop if you break a drill. Handy, especially if you are supposed to tap that hole. Tough work for a tap to run througn a solid carbide drill.

I know if you got a laser tool setter, you can even check form tool profiles.

Next job, I set up, I'll time it to run a few tools, and report back the results. My main thing is that it allows me to do something else while it's probing the tools.

Price out these options from Renishaw, and see where it comes in at.Haas sells the package with a new machine for around $5K. I know I sound like a sales guy, but it works slick. there are a few other guys around who would say pretty much the same thing.
Stang, is it a renishaw tool setter? Maybe you need a different tech guy. Seems to me that the education of the tech guys is not even close to equal.

When we had our machine installed, I spent my training day quizing the guy about what I could do with my probe. He was new to Haas, but he was lucky that he had some prior Renishaw experience.

[stang5197]

Stang, is it a renishaw tool setter? Maybe you need a different tech guy. Seems to me that the education of the tech guys is not even close to equal. When we had our machine installed, I spent my training day quizing the guy about what I could do with my probe. He was new to Haas, but he was lucky that he had some prior Renishaw experience.

Yes it is a Renishaw, similar to what you have where it touches off a "pad" not the laser style.

Yeah he tried the program that was in the machine, but kept getting an error and never could figure it out. He was sharp on everything else.

I am too cheap to call Haas to have them come out and try to figure it out. If you get a chance post a short video of it, I think alot of other people would like to see how it works also.

[Cory]

Originally Posted by HuFlungDung I wish I'd seen the probing thing in action. My noob question would be "How does the machine know when it is anywhere close to where you wish to touch off of, and how does it know which direction to move, etc." I can imagine this taking place in 'slo-mo' but it can't be all that slow or you guys would be complaining about it

It's pretty simple. There's a bunch of different templates for different ways to set your zeros: probe bore, probe boss, probe vise corner, probe external corner, probe internal pocket, etc etc.

All of them have you hand jog the probe to a certain place, for example, if you want to set your offsets to the center of a block, you would handle jog the probe to the rough center of the block, anywhere up to 0.4" above the surface.

Then it'll ask you the x and y dimensions, and the z height above the part. You enter a rough approximation of the size of the block, it starts from center, moves to the left of the block by a bit more than 1/2 of the X value you entered, comes in until it touches off, backs off, and comes in more slowly and touches off again for more accuracy.

Then it retracts and does the same thing with the positive x side of the block, and the + and - Y sides.

You can set your x y offsets and tool offsets in a fraction of the time it would take you to use an edgefinder and gage block/pin/other favorite method.

Originally Posted by Geof So how long does it take to enter the offsets for 10 tools?

It depends if you do length only or length and diameter.

It will only auto sequence length. If length only, maybe 2-3 minutes for 10 tools.

If length and diameter, maybe 2-3x that time.