What's new
What's new

setting tools

Gerrythewelshman

Cast Iron
Joined
Oct 1, 2006
Location
Ireland
Hi all,
This how i set my tool lengths on my mills . I hope it will helps .
You will set many tools in the time you would normally set 1

See photos

1st Z0 setting with taster
1st.jpg


Enter workoffset Z
2nd set hight gauge 0 to Taster 0

2nd.jpg

3rd measure tool

3rd.jpg

enter tool length
 
Just got a used 'taster on eBay.
First thing I did after centering it on the holder was measure the "zeroed" height with my presetter and write the value in black indelible marker on the toolholder.
Now picking up the WCS is a pleasure.
What a fantastic tool the 3D Taster is.

Joe
 
What is your machine doing while you are measuring the tool lengths?
Is it running ?.. or sitting there waiting for the tool?

It also sounds like a lot of ways to make a mistake, you might write the tools length down wrong... you will have to enter those numbers into the correct tool length offset list...and allthe while the machine is doing what?

All I had to do was put a new tool in the tool drum, call it up using the control, move that tool to the Z zero on the part I was making or often I used the machines table as zero, and set the tool on a gage block, then hit SET TOOL LENGTH Button... DONE...NO possible way to make a mistake entering offset numbers and it took me longer to type this than it takes to set a tool up.

But to each hiz own...
 
Hadn't thought of using a taster in exactly that way, but makes a lot of sense to me.

Gary E - on some machines, you have to type the number in manually no matter what you do, so there's an opportunity for error. Further, OP's apporach is much cheaper than a fancy tool setter.

On one of my machines, I use a "tool setter" gizmo which is just a gage that lights an LED when the tool tip is at exactly 2" off the table. That particular machine has "zero here". That is even easier, and pretty error free, like Gary's system. (You can measure tool 33 and tell the machine it's tool 23, and of course Great Unaccuracy results....)

The other machine has a blum tool setter laser, and the machine runs a cycle to set all attributes of the tool. That is very accurate and error free, down to the point of automatically matching the tool number and magazine pocket with the data.

But both of my plans tie up the machine. Gerrythewelshman's scheme could be used in parallel with the machine running.
 
Maybe I should of described the "tool setter" I used... a 1/2 inch gage block... you could use ANY block no matter what it's length, so long as you use the same one all the time.
 
Your scheme has obvious merit (not to mention not requiring batteries.) I like the gizmo with a blinking red light because:

a. I hate sliding a block in and out or using a feeler gage - I'm a computer guy not a feel guy. And dinging the tool or the block is a real hazard.

b. I like gizmos. :D

c. I like blinking red lights.:D

d. I like things that work when I feel sluggish and uncoordinated. :crazy:

e. The gizmo cost less than my first set of gage blocks...
 
Your scheme has obvious merit (not to mention not requiring batteries.) I like the gizmo with a blinking red light because:

a. I hate sliding a block in and out or using a feeler gage - I'm a computer guy not a feel guy. And dinging the tool or the block is a real hazard.

b. I like gizmos. :D

c. I like blinking red lights.:D

d. I like things that work when I feel sluggish and uncoordinated. :crazy:

e. The gizmo cost less than my first set of gage blocks...

a.... Dont do it that way... drop the tool below the block... then slide the block over to the tool, then increment the tool UP until the block slide under... DONE, hit the button and the length is set...

Ohh and another thing.... I never needed a height gage, a fake spindle nose mounted upside down, and a surface plate to mount them all on...

Like I said...this "gage block could of been ANY BLOCK... one of your 2 yr olds toys for all that matter....Just write on it... <<PREC TOOL SETTING THINGIE>>

But youse guys like blinkin lights and and "gizmos"
 
I use two methods,
First is just like Gerrythewelshman's except I use a touch probe instead of the taster with a probing cycle to set the zero. ( I hate wasting time jogging a machine around by hand). My Mits height gage is connected to a computer through the SPC output so the computer sends the reading to my controller.

Second method uses the little light up height setter mentioned by bryan_machine.
I pulled out the guts and connected it to one of my controller inputs. Wrote a small routine so you put the tool somewhere over the setter hit go and the machine comes down and touches off the tool and set the offsets. Also have a program that looks through the part program for which tools will be used then cycles through them one at a time touching each one off on the height setter. A poor man's Reinshaw system.

As I hate having the machine waste time setting tools and not making chips I mostly use method one and setup tools for the next op while the machine is running.

For my uses mostly I'm looking at 8-10 tools with only a 4-5 minute program run cycle so saving time on tool setting really counts.
Bob
 
My setting is similar but I use a fixed "std length" tool. Tool offset is difference between std. tool and cutting tool.

I also never set a Z level on the machine.
G54 Z zero is inside deck of vise, set with the same std. tool.
I then use G10 L2 P0 to transfer x,y, and Z to the program.
Using the deck makes it easy to know where the Z level is without ever being at the cnc.
I haven't set a tool or work offset at the cnc for 7 years.
 
tool setting

Hi,
I to have used different ways to do this.

Advantages

you can run the machine whilst setting tools.

You will have the taster in for X Y anyway

All tools in the carosel will be done this way

You can touch off Z at any hight for multiple work offsets as all tools are set to it
 
I use a very slightly different method
But then I would :nutter:

I use one of these
Probe1.jpg


In combination with a table mounted tool probe like this

ttprobe.jpg


The edge finder is set up carefully with some 135 mm slips on the bed, and a tool length of zero, the 135 mm height was picked because it is also the center line of the 4th axis.
The Z axis is wound down so it reads zero and the edge finder is carefully mounted so the slips just go under it.
This then calibrates the table mounted tool probing thingy(technical description there ;))
Then its a simple matter to touch off the tools on the probe as needed.
You only need to do the calibration routine once, since if you smack the edge finder into a part and break it :bawling:, you only have to reset the length with the slips. :cool:

Boris

Now if only my boss would buy some more tool probes since I've only got the 1........ :(
 
If you are worried about setting the tool's offset as the wrong offset number by accident (tool 1's length as tool 10) or worried that you got dyslexic and put in the wrong number, then here's how I check my tool offsets.

I make a simple program that I can use to send the tool to 1.000" above my G54 Z.

EX:


T1
M6
M00
(MAKE SURE TOOL HAS OFFSET IN OFFSET PAGE - THEN CONTINUE)
G90G00G54X0.Y0.
G43Z10.0H01
G01Z1.0F75.0
M00
(SLIDE 1 INCH BLOCK UNDER TOOL AND MAKE NECESSARY ADJUSTMENTS)
G91G28Z0.0

and you can copy and paste this block of program for as many tools as you are going to check, just change the T# and H#

The company I work for uses a tool setter in the tool crib, but seeing as I work with a bunch of button pushers and people who lack any kind of skill, I have to make sure to double check things.


always...

and then I have one of those bosses who will say things like..

"Just go with what the tool crib gave you for offsets, you're wasting time checking those, just load the tools and go"

then when you get a nasty mismatch or one of the numbers was just off by like .100" or something he'll say

"The number the tool crib gives you is just a reference number, this isn't acceptable."

SO anyway, I have to find fast ways to check tools before my boss can bother me about it and that's how I do that. I'm sure most of you guys already know about that as it's somewhat common sense, but to anyone who never thought of it, I hope it helps.
 
a.... Dont do it that way... drop the tool below the block... then slide the block over to the tool, then increment the tool UP until the block slide under... DONE, hit the button and the length is set...

I do it the same way. 1" gauge block, drop below, and bring the tool UP (not down), until it slips under, then type the absolute Z into the offest table (adding 1"). If I'm using parallels, i set the tool using them directly, and don't add the 1"......
 
I do it the same way. 1" gauge block, drop below, and bring the tool UP (not down), until it slips under, then type the absolute Z into the offest table (adding 1"). If I'm using parallels, i set the tool using them directly, and don't add the 1"......

I do something very similar using the 1" block and I also move UP to set the offset. I go one step further and use one of my fixture offsets (G58) to set absolute zero on top of that 1" block. The absolute display reading is then transferred into the offset table using "Z input" so no typing is involved.

This is on my old Fanuc 6MB control.

Our newer Haas machine use the Renishaw probe.

Two thoughts about this system:

1. I hate having to write a program to touch off each tool length.

2. I cringe every time I see that tool headed down onto the probe button, although it has never caused any problems so far.
 
:typing:

It occurs to me that part of how I do things is because (a) I was making it up as I went and (b) some features of my first mill never did work, so I took a discount and went on. The automatic tool setter hooked to the controller was such a feature. (The machine does have a very nice integrated probe which cost about 1/10th what a renishaw does.)

Of course, as with any formal tool setter, all you really need is a fixture that let's you calibrate a height gage to read zero at the gage line, and away you go...

Now the bit where I wonder if what is do is so far far away from production shops....

On both my machines, once a tool's height is set, it may be checked for paranoia reasons, but in general doesn't change until it breaks or wears out, and that happens fairly rarely. So I try to build a "set of all needed tools" so that many pieces can be made without touching anything off.

It sounds like several of you have to touch a bunch of stuff for each job. Is this because you wear stuff out faster because you make way more parts? (I've never made more than 12 of any one thing.) Or do you have way more tools than holders? Or?
 
I have used a Taster for about the last 10 years.

When I first got it, everyone in the shop thought I was crazy for spending almost $500.00 on an edge finder. Then after they watched me use it for about 6 months and saw how fast it was to find the edges of a part or the center of a hole everyone wanted to borrow it.

I just told them where they could buy one.

I had another device that I used to set the Z height of my tools which was equally as fast. I can't remember what it's called, but it was 1 inch tall and on the Haas after you get all the tools set, you just go to your G54 and tell it to go Z-1.0000 and you were where you wanted to be. Very fast. Touch tool, dial to zero, measure Z offset, next tool and you're done.
 
Gerrythewelshman,

I use almost the same method you use, except I don't refrence the tools off the taster at zero. I would be confused with positive and negative lenghts for tools.

Why not zero your height gauge off the face of the "spindle" on your fixture, and measure all the tools as positive numbers from there. Then measure your taster at zero in the same fixture, also a positive number. Then insert taster into mill spindle and move to the top of the part, and insert the number you get on the mill z axis (usually a negative number) into your work offset for z and subtract the lenght of the taster (make the negative number in the work offset bigger by the lenght of the taster). That way all tools are positive measurements from the toolholders gauge line, and the work offset is a negative number, the distance from the mills gauge line to part zero.

I like this method the best. I only have to measure the taster once and the tools are always the same lenght unless I break them down. If I take them out of the machine I put a post it note with the length on the tool. That way I don't have to measure it again the next time I use it. If I'm using vises I just set the work offset z zero off the bed of the vise and write that number down on a post it note. Then I add the height of the parallels and the part to the workoffset. That way I can change parallels and parts and I can adjust the z work offset without having to touch off on each setup.

I also measure tools while the machine is running to save time. Besides our newer mills alarm if you jog faster than 10% of the rapids with the door open, which makes setting tools take forever. On my okuma I can also put the tools into the carousel and enter the tool/pot numbers and tool offsets while the machine is running saving more setup time.

Gary E

I used to use your method but found it to be slower and not as accurite. There is no way to set tool lenghts to tenths with a gauge block or piece of paper. I was getting steps on pocket floors that I used multiple tools on. With the tool presetter I get perfect blends between multiple tools on the first shot.
 
Gerrythewelshman,
There is no way to set tool lenghts to tenths with a gauge block or piece of paper.

I beg to differ, on occasion I have to hold tolerances like this at work on a mill. Using a ground 1" block and feeling for when the tool starts to barely make contact. To clarify I wasn't holding plus or minus tenths but plus or minus one thousandth. It all depends on how much backlash your mill has and how good you can feel the drag on your block. I agree with the statement about paper though. You shouldn't really ever use paper unless you are goofing around or setting a drill tip to 0 off the top of a block or something. Anyway, that's just my 2 cents....;)
 
Another benefit to Edster's way is you can put any tool in any machine and the length is the same. It also let's you measure the next tools for the next job while your still running the current job.

Also you can use any tool to set your work height.

Over the years I have used most methods discussed here. I find the positive length from the spindle nose the best for me.

If I had a table mounted in machine pre-setter then maybe I would think different.

One method that I like the least is where each tool is touched off on the part.:willy_nilly: This is the method that I was taught when I started CNC usage. Now that I have seen the light I just don't like that method.

To each is own.
 
I beg to differ, on occasion I have to hold tolerances like this at work on a mill. Using a ground 1" block and feeling for when the tool starts to barely make contact. To clarify I wasn't holding plus or minus tenths but plus or minus one thousandth. It all depends on how much backlash your mill has and how good you can feel the drag on your block. I agree with the statement about paper though. You shouldn't really ever use paper unless you are goofing around or setting a drill tip to 0 off the top of a block or something. Anyway, that's just my 2 cents....;)

I use one of these Lyndex-Nikken Products

It takes less than 30 sec to measure a tool and write down the measurement in length and dia. It's good to 5 microns in the z that's about .0002, how long does it take to measure the tool with the block? Btw I used to use the block/paper method until I got tired of making small adjustments to the length to get to target, or to get two tools working on the same pocket to blend on the floor.

For the guys that think measuring on the machine is as quick, did anyone even consider the time that it takes to adjust the tools or just the time for the initial measurement.

IMO you can't beat using a presetter to measure tools. And the best part is one presetter can be used to measure tools for all the mills in the shop as long as the tapers fit the presetter.
 








 
Back
Top