Touch-off tool length offset setting locations for milling machines & VMCs

[PhoenixMetal]

I set up my tool length offsets using the "touch off" method using an electronic contact indicator (it lights up when the tool touches it) on my Vertical Machining Center. Normally I rest the indicator on (and therefore set my part z zero point relative to) the top of my workpiece.

This has been working great so far, however I came to realize a limitation of this technique for some parts: What if the part I am making no longer has any flat surface at the original z depth to set to after some machining operations, and I break a tool and have to replace it? I'd be out of luck in that case!

So, I've been thinking of always using the top of the fixed jaw on the vise as my new point to zero tools from, and I would compensate for the true location of part Z 0 either via my G54 offsets, or within my CAM software. Doing this would also be nice as it would eliminate re-setting the offsets for every different part that I make. I would only have to make one global change for the part height above (or below) my reference level (top of the the vise fixed jaw).

I was wondering what some of the more experienced folks out there do about this... Is my proposed tool setting location something that is commonly done? Does it work well? Is there yet something even better that I may want to try instead?

Thanks in advance for your input!

[Geof]

What you are proposing doing is fairly standard; chose a location that stays there and touch off from that, then have a value for Z in the G54 or whatever work coordinate you are using.

This has been discussed before and my contribution has always been:

Make your touch off position higher than your highest job. This way your Z values in the work coordinate a negative because you have to come down to the job. The reason I suggest doing it this way is that if a mistake is made and a positive value is entered then the tool goes too high and nothing interesting happens.

If you make you touch off point lower than the job then the Z value has to be positive. If a mistake is made and a negative value is entered then your tool goes tool low and lots of interesting things might happen.

[PhoenixMetal]

Hi Geoff, thanks for your input. Good to know that this is a common technique.

Your suggestion to keep the touch-off position higher than your highest workpiece is smart as it can help avoid crashes, however unfortunately, most of my parts stick out of the top of my vise, and the vise is the tallest object that is (nearly) always present.

Thanks!

[Geof]

On one machine we bolted a length of round bar to the table just within the machines limits and on a lot of others we just use a 6" high gauge block.

[PhoenixMetal]

It sounds like you really take your crash prevention measure seriously... Maybe I should too. I think using a gauge block would work best for me as I'd rather not have an extraneous item always on the bed. Maybe just for appearances sake. I guess a purchase of some 2-4-6 blocks is in my future!

[Geof]

Originally Posted by PhoenixMetal It sounds like you really take your crash prevention measure seriously...

We do.

It pays off; I think being at home so none of the machines can hear me it is safe to get cocky. We do pretty good in the matter of crashes; we have not had a spindle to vise or table crash ever and I think the last toolholder to fixture crash was about three years ago. This is with 20 machines.

[skip56uk]

Originally Posted by Geof What you are proposing doing is fairly standard; chose a location that stays there and touch off from that, then have a value for Z in the G54 or whatever work coordinate you are using. This has been discussed before and my contribution has always been: Make your touch off position higher than your highest job. This way your Z values in the work coordinate a negative because you have to come down to the job. The reason I suggest doing it this way is that if a mistake is made and a positive value is entered then the tool goes too high and nothing interesting happens. If you make you touch off point lower than the job then the Z value has to be positive. If a mistake is made and a negative value is entered then your tool goes tool low and lots of interesting things might happen.

This does work...... but i got a better way !!!!!!!!! lol

I wrote a macro that rewrites my tool offsets.
My offsets are allways a - figure fron the spindle nose.
all tools set of post on table that never moves.
the offset for T99 the nose to top of setting post and thats what the macro works from.

similar to a renishaw probe.

you macro should look somthing like this ....

%
N010 O9999 (TOOL SETTING MACRO)
N020 ()
N030 #CLEAR
N040 ()
N050 #PRINT "ENTER START TOOL"
N060 #INPUT V1
N070 #PRINT "ENTER FINISH TOOL"
N080 #INPUT V2
N090 M0
N100 #PRINT "PRESS START"
N110 #V1=R1
N120 #V2=R2
N130 ()
N140 #:START
N150 ()
N160 ()
N170 T+R1 M6
N180 M0
N190 #PRINT "JOG TOOL DOWN TO CLOCK 0. FROM BED"
N200 #PRINT "THEN PRESS START"
N210 ()
N220 #IF TN=1 THEN GOTO :TOOL1
N230 #IF TN=2 THEN GOTO :TOOL2
N240 ()
N250 ()
N260 ()
N270 #:TOOL1
N280 #H1=H99-AZ
N290 G0G90
N300 H0 E0 Z0.
N310 #R1=TN+1
N320 #IF TN=R2 THEN GOTO :STOP
N330 #IF TN<R2 THEN GOTO :START
N340 ()
N350 ()
N360 ()
N370 #:TOOL2
N380 #H2=H99-AZ
N390 G0G90
N400 H0 E0 Z0.
N410 #R1=TN+1
N420 #IF TN=R2 THEN GOTO :STOP
N430 #IF TN<R2 THEN GOTO :START
N440 ()
N450 ()
N460 #:STOP
N470 M30
%
%

this is only part of the macro
for tool 1 and 2 only and was writen for a fadel.

if any body would like some help with macros dont be shy and just yell at me ok

[ALLtra Mach]

Phoenix,
On VMC's, and really all machines for that matter, there are 2 basic ways of setting tool lengths. It is either a distance from home to Z0, or your fixed measuring point which is what you guys are discussing, or it is the actual length of the tool. I use the actual tool length method for a couple of different reasons. First being that in a high production shop, your tool lengths can be measured and set offline.

[PhoenixMetal]

Hey guys, I've started using a single fixed position to set my tool lengths now with a just my G54,G55 etc. offsets to set the part height. Man this is saving so much time! I can't believe I didn't know to do this earlier!

Granted, I had never even seen a VMC in person prior to buying one, but I read a whole lot during my learning process, and nowhere did I find this really important tip written. Thanks for your help guys!

[Cartierusm]

I thought with VMC you use a fancy, and expensive, fixture holder and it helps set the tool in the mount exactly at the same length? So if you break something you reset it and the tool is perfect?

[Geof]

Originally Posted by Cartierusm I thought with VMC you use a fancy, and expensive, fixture holder and it helps set the tool in the mount exactly at the same length? So if you break something you reset it and the tool is perfect?

Not exactly; the length of the tool has to be measured somewhere.

In a big operation with a proper toolcrib you may have a tool pre-setter which measures the distance from the tool tip to the gauge line on the holder; It is impossible to install the tool at a specific distance accurately enough so it is measured afterwards. Then this measured distance is used to set the offset for that tool in the machine without needing to actually measure it in the machine.

When the tools are not prepared beforehand and measured in a presetter the tool offsets have to be determined with reference to some point in the machine. You can do it almost anyplace but it is probably more convenient to have a fixed reference point as has been discussed.

[Boots]

We made presetting blocks for the different machines. We use an Indexer on most of the machines and the rotary indexer center height is different on every machine. So we set our tools there and the program for machining is figured from the center of the part. We started out programming from the top of the stock but if a tool breaks and the part is no longer round there is no way to set it because the reference surface is gone. A tool setting block was the only answer.