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.

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 :D

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.

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.

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 :D

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!

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?

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.

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" :-(

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.

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.

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 :D

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.

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.

Thanks for the info guys :)

You can insert the macro calls for position into the programs if you required to pick up datums for every part, if you so desired, say if you were working with castings and such as well. You are pretty much limited by your imagination, as to what you can do with the probe, well your imagination, and your ability to write the associated macros.;)

what ive worked with for a couple month that was ideal , was a bench top tool presetter , the tools not set from the reference point but the actual tool length is punched into the tool page manually ,the part is probed and the w/s is always a negative , the benefits of using the presetter is while one tool is running the other one is being set , once the tool stops the next tool is ready to go , also the presetter can be used for checking the tools for runout on the side of the tool as well as the bottom of the tool , it also works great for clocking in a boring head within a couple thou then only having to tweak it in the machine ,
nice tool bit pricey but in my opinion well worth it

As far as the Haas tool setter goes, It works great takes a couple of minutes but it knows through parameters where the touch pad is and moves to position and calls up the tools and touches them off and sets the offsets. really cool and fast. Stang call Haas and ask which probe system you have if its renishaw code they will tell you over the phone how to get it going. I've used Hitachi's with probing and they actually read the program call up the tools from the program and set them accordingly to the h numbers in the program very easy. I've also used lasers on matsurra horizontals so accurate and easy I didn't trust it for at least 2 set-ups and once its set you can use any tool in the machine on any part and it will always work their is a master tool you set off the tombstone for what ever fixture face your using or part face. and it sets it in your work coordinate. The macro program is really easy to understand just download the instructions from renishaw read them three times and you will get it. like with the haas you can set a height to start the initial probe say 4" above the probe depending on tool length differences then it feeds at a feed rate you set say 50 ipm then 20 ipm then finally a couple inches per minute all the while it varies its start point based on the initial hit. so there is not much time wasted. Geof on your set up do you leave the indicator on the machine? if not what happens if somebody moves the dial or indicator when you go to touch a broken tool? It seems like a great poor mans solution I'm just curious about repeatability.
Joe

.....Geof on your set up do you leave the indicator on the machine? if not what happens if somebody moves the dial or indicator when you go to touch a broken tool? It seems like a great poor mans solution I'm just curious about repeatability.
Joe

They don't stay in the machine. When a tool is replaced and touched off the one adjacent is touched off to compare and see if the Toolsetter is truly back in the same place. That is the reason for the comment about coolant films making a difference. Repeatability is +/-0.0005 without taking much care and better if you try. Ten offsets take 3 or 5 minutes to enter. You are 180 degrees out of phase with your poor man's solution.

My thing is when you are seeting these offsets manually, you need the dood there all the time. with the Renishaw, when it runs, I can be doing something else at the same time whether it be clean up the bench, get my fixtures ready or put away, get the material ready, use the washroom. All while most of the tools are getting set.

.....with the Renishaw, when it runs, I can be doing something else at the same time whether it be clean up the bench, get my fixtures ready or put away, get the material ready, use the washroom. All while most of the tools are getting set.

This was my question;

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

This was the answer:

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

If you can do everything you mention I want you working for me; such efficiency I have never seen. Crikey I need more than the three minutes in the washroom...or is that just an age thing?:D

we are still in the stone age i guess. dont laugh, but........... yes i still use paper. lol

we are still in the stone age i guess. dont laugh, but........... yes i still use paper. lol

Nothing wrong with that! The technique I described is what my guys do, I use paper or when the top surface is going to be faced I just turn the spindle on and bring the tool down until it starts cutting.

What always impresses me is the thickness quality control on paper. I guess in relative terms it is poor because it will vary +/-25% but that is +/- about 1 thou.

Geof

The only thing I want to add to your original post is that the Zd does not have to be negative, and your Work Z0 can actually be above Z-home.
Unfortunately on the MiniMill sometimes it is a necessity due to the incredibly short Z travel.
My Z0 workoffset is often positive as I use a 2" tool setter on the table surface, while my parts are in the wise, usually 1 or 2" above the top of the toolsetter.

Geof

The only thing I want to add to your original post is that the Zd does not have to be negative, and your Work Z0 can actually be above Z-home.
....

That is perfectly correct.

We do not make Zd negative because the machine needs it to be negative.

We make Zd negative because I say so and I am the Boss.

There is a reason for this:

If Zd should be positive and by mistake you fat finger it and put in a negative...which is very easy to do...your tool goes 2*Zd down into the work or vise.

If Zd should be negative and you put in a positive all that happens is you machine air with the tool 2*Zd too high.

I prefer mistakes that machine air, much cheaper than vises. :)

Paper is where it is at!!!!!!!!! I use it and love it. $100,000 machine, $0.03 Tool offset device. : )

I guess you're right in that regard.
I know from experience that very few fat fingered mistakes come out good, this may be one of them though.

Tony

What happens when you sneeze or someone yells "Look Out" right next to you while cranking the handwheel onto the $.03 toolsetter?

Paper is where it is at!!!!!!!!! I use it and love it. $100,000 machine, $0.03 Tool offset device. : )

Do you use Haas? Although I guess this comment could apply to other machines. The Handle Jog wheel has a little knob on it and when we (this is me and my guys) used paper sometimes when reaching for the jog handle we would bump the little knob and give the spindle a nice quick negative move of 50 thou or so and wipe out a brand new $100 tool by chipping the end as it rammed into the job. The toolsetter can handle about 0.15" over-travel.

I was being mostly sarcastic but I have had the LOOK OUT! BS uttered in my shop while paper was the tool offset device. Usually resulted in a nice expensive bill and an argument with the ass that has the big mouth. : )

LOL Cheap ass people get with the time and buy a presetter and stop living in the stone age... by the way I do still use paper some time but only for the sentimental value. heheheheh d-_-b

On a serious note what has always work great for me and it gets all my guys on the same page is that we take all the offsets on the table. Not only does it keep the consistency on the tooling specially from job to job but it make it easier on everyone to touch off tools. The added bonus is that by using the Z value on the work coordinate then you can use the same tools you used on the last job. The only thing you need to do is change the Z value in the work coordinate and that beats the hell of trying to either touch off all the tools again or manually alter their value if you know the height differential.

I just found this forum and thought I would add my two cents into this as I find this to be a problem in many shops.
I have used tool setters in and out of the machine to include a lazer tool setter as well.
I have found that using this methods works as well or better then many high dollar items especially the tool setter out of the machine.

Using a 123 block or even a 246 block to locate on a clean surface of the table, bring down your tools below the height you wish to use and raise in .001 and later to .0001 to find the Height Offset as we know using a Haas makes this very easy, then use a Test indicator not a travel indicator touch off the block and Zero your Z, then move to your Work Z Zero location and insert this number into your Z Work Coordinate.

Depending on your care you will eliminate the majority of your blending problems and dimension requirements.

There are those that will say well that is close enough on their setups and they usually will find they are fighting to keep their part into tolerance after the 3 or 4 operation, tolerances are used for production not in programming or setup.
Build that strong foundation and eliminate all those problems ahead of time.

note: when touching off face mills or larger endmills there will always be one tooth lower then the rest.

If my work coordinate system is G54. Are all my offsets taken when that system is active? And is the z difference between the top of the workpiece and the tool also entered in the z on the G54 line? Does G129 come anywhere into play?

If my work coordinate system is G54. Are all my offsets taken when that system is active? And is the z difference between the top of the workpiece and the tool also entered in the z on the G54 line? Does G129 come anywhere into play?

G129 is just another work zero so if you are using G54 then G129 is not in use.

Your tool offsets can be taken directly to the top of the workpiece which means that nothing goes in the Z column for G54, or any other work zero.

Or your tool offsets can be taken to some reference point, the top of the vise, a block on the table, etc. Then the difference between the height of the reference point and the top of the workpiece goes in the G54 Z value, you have to enter this by hand.

In my shop we very often use a reference point and we always make sure it is higher than the work piece. The reason for this is that then the Z value is negative; if someone makes a mistake and enters a positive Z value not much happens b ecause the tool then goes too high.

If your reference point is below the top of the workpiece then the Z value has to be positive. This time if a negative value is entered by mistake then the tool goes too low and this can be serious.

G129 is just another work zero so if you are using G54 then G129 is not in use.

Your tool offsets can be taken directly to the top of the workpiece which means that nothing goes in the Z column for G54, or any other work zero.

Or your tool offsets can be taken to some reference point, the top of the vise, a block on the table, etc. Then the difference between the height of the reference point and the top of the workpiece goes in the G54 Z value, you have to enter this by hand.

In my shop we very often use a reference point and we always make sure it is higher than the work piece. The reason for this is that then the Z value is negative; if someone makes a mistake and enters a positive Z value not much happens b ecause the tool then goes too high.

If your reference point is below the top of the workpiece then the Z value has to be positive. This time if a negative value is entered by mistake then the tool goes too low and this can be serious.

I've been setting all my tools to the top of the workpiece (my zero). But now i'm trying the method you describe, so the sequence I'm doing is indicating my block to get x0.0 and y0.0 in G54, then I touch all my tools of to my gage which is higher than the workpiece (still in g54) and press the tool offset and next tool till i'm done with all the tools. now how to establish z0.0? I know you said measure the difference between the tool and the top of the workpiece. Do I zero out the z column then manualy put in the difference or do I touch a tool to the top of the workpiece and enter part zero?

I just realised I am getting old and senile; this is my thread!:D

I describe my procedure in detail in the first post that started the thread.

Nothing wrong with that! The technique I described is what my guys do, I use paper or when the top surface is going to be faced I just turn the spindle on and bring the tool down until it starts cutting.

What always impresses me is the thickness quality control on paper. I guess in relative terms it is poor because it will vary +/-25% but that is +/- about 1 thou.

In the begining years I used paper to but one slight Oooops lead to chipped end mills so I switched to Plastic Shims. You can get a whole book .001-.03 for about $20. They work great and depending on what Shim you use you have some a little room for error.

The shops around here are too cheap or ignorant in efficient equipment, lol, bean counters. :)

I like this presetting process though. Thanks for another great Thread Geof!!. :)

I've been setting all my tools to the top of the workpiece (my zero). But now i'm trying the method you describe, so the sequence I'm doing is indicating my block to get x0.0 and y0.0 in G54, then I touch all my tools of to my gage which is higher than the workpiece (still in g54) and press the tool offset and next tool till i'm done with all the tools. now how to establish z0.0? I know you said measure the difference between the tool and the top of the workpiece. Do I zero out the z column then manualy put in the difference or do I touch a tool to the top of the workpiece and enter part zero?

Bob, Not to make things a bit confusing but I think you need to understand the concept of work offsets. a G54 for example is a local coordinate you already set the x and the y for the reference of your block, you dont need to be in any particular setting to set the values for local coordinates, if you wanted to set G55 in the oposite end of the vise and you knew the value, you could just punch in the numbers so theres nothing to it. Now to the meat of your question LOL... The Z value on you Local coordinate i.e G54 will shift the value of all your tools height offset by whatever number is applied into G54. Please beware as Geof said That Value can either be positive or negative, whatever point you are using as reference, if you have more than one person working in the machine, once you developt whichever process for set ups.... Make sure everyone is on the same page. Ps: By the way in case you wonder if a tool brakes, you still touch the tool in the same location as the other tools and it's value will be shifted by whichever Local coordinate system you will be using. Best of Luck

ok, thanks for your patience, but I'm doing something wrong. Here's what I did yesterday and it worked, this morning I added a new tool and that height was wrong. Here's what I did, please tell me where I went wrong.

1) established my x and y zero
2) touched off six tools to my gage above the workpiece
3) took tool 1 and touched it off to where my z zero on the workpiece is and for the z column in g54 hit part zero
4) took the tool offset value for T1 and subtracted it from the z column
5) everything was fine all tools were at the right height. program ran great.

6) this morning needed to add another tool (t7) I touched it off my gage block and selected tool offset measure. Ran the program and that tool was at the wrong z height.

Bob, Im a bit lost.... Are you using a touch probe ??? Ok whatever you used on top of your work piece you know the value of it right ? That's the only value you need to put in G54. Say you touch off all the tools on top of the part using a 1 inch gage block, in your G54 or whichever one your using you will have the value on your X#### Y#### Z-1.0 <~~ that is the value you need to add as long as you are touching above the part it will be Z-####
You dont need to touch off tool number one and do the math and all that crap. You only need to do that when a probe is involved. Hope this helps Bud:)

Bob, Im a bit lost.... Are you using a touch probe ??? Ok whatever you used on top of your work piece you know the value of it right ? That's the only value you need to put in G54. Say you touch off all the tools on top of the part using a 1 inch gage block, in your G54 or whichever one your using you will have the value on your X#### Y#### Z-1.0 <~~ that is the value you need to add as long as you are touching above the part it will be Z-####
You dont need to touch off tool number one and do the math and all that crap. You only need to do that when a probe is involved. Hope this helps Bud:)

I fully understand what your saying however, It didn't work. The way i oringinally tried was I touched all my tools to my gage(indicator in housing on 123 blocks) hit the tool offset measure button, next tool and so on. I measured the height difference from my gage to the zero on my work piece ( the value happed to fall exactly 1.360) I then entered -1.360 in the z column and ran the program and it was not right. The only way I got it to work was to set tool 1 to the my workpiece zero then hit part zero in the z column and then subtracted the height offset value ( i think it was 2.887) for that tool.

ok, thanks for your patience, but I'm doing something wrong. .....


6) this morning needed to add another tool (t7) I touched it off my gage block and selected tool offset measure. Ran the program and that tool was at the wrong z height.

Yes, this is what I warned you about.

There is a Setting 64 Tool Offset Uses Work Zero, read the manual for a description.

When it is ON the value in the G54 Z is subtracted from the Z distance that is entered. The value entered is the tool offset distance in G54.

When it is OFF the the machine coordinate value is entered.


The procedure you described is equivalent to mine; the reason I use a toolsetter and dial gauge is simply because it is possible to chip tools touching them off directly.


Paulo E; You are correct, ifyou have a gage block of known thickness actually resting on top of the workpiece, but if the touch off block is in a different location it is necessary to get the difference in Z between the block and the workpiece.

Bob there's only 2 things I can think of as to why one of the tools would not work or in a particular case all the tools, Please check you are using the correct local coordinate in the program make sure if you are using G55 that, G55 is what you have in your program and the other thing is check to make sure you have the g43 posted out with the right H value for example T1 H01. Im a bit tickle by it now if you have all the settings correct and you still have a problem, then if u dont mind post your email and see if we can comunicate and I can help you out

Bob there's only 2 things I can think of as to why one of the tools would not work or in a particular case all the tools, Please check you are using the correct local coordinate in the program make sure if you are using G55 that, G55 is what you have in your program and the other thing is check to make sure you have the g43 posted out with the right H value for example T1 H01. Im a bit tickle by it now if you have all the settings correct and you still have a problem, then if u dont mind post your email and see if we can comunicate and I can help you out
I am using g54 and I do use g43 with the matching T and H value. I am looking at the setting that Geof had mentioned, I think that could be what's throwing me off.

Yes, this is what I warned you about.

There is a Setting 64 Tool Offset Uses Work Zero, read the manual for a description.

When it is ON the value in the G54 Z is subtracted from the Z distance that is entered. The value entered is the tool offset distance in G54.

When it is OFF the the machine coordinate value is entered.


The procedure you described is equivalent to mine; the reason I use a toolsetter and dial gauge is simply because it is possible to chip tools touching them off directly.



Paulo E; You are correct, ifyou have a gage block of known thickness actually resting on top of the workpiece, but if the touch off block is in a different location it is necessary to get the difference in Z between the block and the workpiece.

Thanks Geof, that was the setting that threw me off. Everything is working as it should not.