[panaceabea]

I am having a little trouble figuring out the routine for setting tool length offset on the new Haas mill. I am new to haas but not machining, TLO on my other two mills is a simple single button setup from the jog page, touch the top of the block(of known height) with the tool , push the tool set button and its done .

I have followed the HAAS manual to a T (I Think) but I am guessing there is something simple I am missing or have screwed up. Here is the procedure I am following as best I understand it from the manual, page 58.

g54 z value is 0

load tool in the spindle

enter jog mode

jog tool down towards tool setter (gauge block in my case)

touch off on block

press ofset

page up until I am on geometry for the tool in the spindle

press tool ofset measure

press next tool

load next tool in spindle

touch off repeat etc .


All seems well and it loads the machine z position -**.*** shown into the tool table , the problem I am having is none of the tools are set at the correct offset .
When load the individual tools thru M06 T** and go back and check them for refrence against the gauge block none of them are set at the same place.
One of them , always the 1/2 endmill , no matter what T number is assigned to it , is always exactly at the top of the tool block but all the rest are at different hieghts.

They range from being almost an inch above the block to -1.2" (1.2" Below the top of the block)

I am sure I am just missing something simple here , the process seems simple enough once I figure out what I am doing wrong .

[behindpropeller]

I am having a little trouble figuring out the routine for setting tool length offset on the new Haas mill. I am new to haas but not machining, TLO on my other two mills is a simple single button setup from the jog page, touch the top of the block(of known height) with the tool , push the tool set button and its done .

I have followed the HAAS manual to a T (I Think) but I am guessing there is something simple I am missing or have screwed up. Here is the procedure I am following as best I understand it from the manual, page 58.

g54 z value is 0

load tool in the spindle

enter jog mode

jog tool down towards tool setter (gauge block in my case)

touch off on block

press ofset

page up until I am on geometry for the tool in the spindle

press tool ofset measure

press next tool

load next tool in spindle

touch off repeat etc .


All seems well and it loads the machine z position -**.*** shown into the tool table , the problem I am having is none of the tools are set at the correct offset .
When load the individual tools thru M06 T** and go back and check them for refrence against the gauge block none of them are set at the same place.
One of them , always the 1/2 endmill , no matter what T number is assigned to it , is always exactly at the top of the tool block but all the rest are at different hieghts.

They range from being almost an inch above the block to -1.2" (1.2" Below the top of the block)

I am sure I am just missing something simple here , the process seems simple enough once I figure out what I am doing wrong .

Great post. I am having the same problem. I have a hard time following the manual.

Tim

[Geof]

That is puzzling. I normally load all the tools first then go back to the beginning and do the offsets:

Touch off tool on gauge block

Push Tool Offset Measure

Push Next Tool

repeat for all the tools.

That is no different to your procedure so why doesn't yours work.


No values in any work offsets you say so the Setting that selects for subtracting the work coordinate Z value from the tool offset should not be doing anything.

Check that Setting anyway. I cannot remember the number but it is called something like TOOL OSET MSR USES WORK ZERO.

Have you tried entering the tool offset value from the keypad? Touch the tool, type in the Z position at the bottom of the screem and press write. Do you get the same value entered this way?

It is sure to be something ridiculously simple.

[panaceabea]

Have you tried entering the tool offset value from the keypad? Touch the tool, type in the Z position at the bottom of the screem and press write. Do you get the same value entered this way?

Yes I have tried entering it manualy, same number, same problem,
I am going to call Haas tech in a few minutes and will update with what I am doing wrong

[panaceabea]

still not sure what I am doing wrong , the fellow explained how I need to enter the distance from the top of my touch off block to the table as a positive number in g54 z position before touching off and pressing measure tool offset key but it still hasnt solved the problem of tool offsets being wrong .

Check setting 64 for the "use work for tool offset" and its off .

[lkenney]

I set all my tooling to a 2" dial gage block, then change the G54, G55 etc Z axis for the different parts that we are machining.

I bring up the Offset screen which on my machine is 1-15 tools, have to flip to second screen for T16, install a tool in the spindle, crank down to the gage, could be a 1 2 3 block or the top of the vise, set tool to a standard zero on the gage or setup block, push tool offset and i am done with that tool.

When I load a program and then the first part, I load from the TC an end mill, bring it of the part somewhere that will be cut away if possible and running at about 1000 rpm bring the tool down to just touch the material usually only a very slim arc. I then subtract the tool zero length from the current tool height and page up the the part zeros and put in the calcualted offset in the G54-g55 etc Z position.

If I don't want to mark the material i will use a gage block, feeler gage or a piece of paper to get the tool close and subtract out the thickness of the block or feeler gage. The tool is not running when I take the measurement with these tools


Eagle

[panaceabea]

Thanks for the input, I am not debating the method by which we all touch off or otherwise measure TLO , the problem I am having is that when I push the measure tool length button it enters the number in the tool table, but none of the tool lengths (other than the .5") are correct

[behindpropeller]

Thanks for the input, I am not debating the method by which we all touch off or otherwise measure TLO , the problem I am having is that when I push the measure tool length button it enters the number in the tool table, but none of the tool lengths (other than the .5") are correct

Check your setting 64. I can't find the thread on if it should be on or off without a toolsetter.


Tim

[HuFlungDung]

This 1/2" holder you say is always correct when measured. Even in a different pocket?

Any chance of some kind of mixup between metric/inch?

What is the machine Z position readout at the Z home? What is the Z position with the spindle nose touching the gauge block sitting on the table?

There's got to be a way of systematically discovering the error by measuring tool lengths to gauge line (use a height guage and a socket on the workbench), calculating what the length offset should be, then comparing those results with what the machine seems to be measuring.

[lkenney]

Are the tools constantly off length? Please give us some actual numbers to work with. ie: tool one is measuring ____ length but when used is cutting xx" low or what ever is true.

Eagle

[panaceabea]

I am at somewhat of a loss on how to proceed. I have cleared the tool library in an attempt to start over , the machine says tool 5 is in the spindle so I have insterted a 1/2" endmill in the spindle and homed the machine . readout says x0.00 y0.00 and z0.00 as expected. My tool setter is 5.00" off the table . When the 1/2" endmill is resting on the tool block the z axis reads -18.7601 . pushing the tool length offset measure button then enters that number in the length geometry box for tool 5.

At this point the manual indicates I should push the next tool button to advance to the next tool, I get an invalid tool number error message and cannot proceed. As there are no other tools entered in the tool library I cant callout m6 T** to advance . Not sure how to get the machine to put tool 5 back in the carousel and let me load the next tool. Worked earlier using the next tool button as described in the manual

[lkenney]

If I am putting a whole series of tools in order I load the first tool (usually t2 as i like to keep tool 1 open if i can) then put the tool in the spindle and measure it, then push ATC FWD which will take the put the tool first tool in the ATC and advance the ATC one tool, repeat until you are loaded. If I am putting in select tooling then I hit the MDI button key one time so not to invoke DNC and key in "T6" or what ever tool I want to work with then punch either the ATC Fwd or ATC REV button.

Should work for you.

Let us know.

Eagle

[panaceabea]

trying it now with just two tools of know length, will post hard numbers in just a minute

[lkenney]

You are using a side mount Tool changer and I am not. Sorry I have never used one. I don't know how they work, but it seems to me that at a Haas show locally I was shanging tools on a VF2 just by pushing the ATC FWD button. Sorry you will have to get someone with new equipment than mine to help you. Call Haas or your local dealer and have them talk you through it. They are there to help and you can't make chips without it working.

Good luck.

Eagle

[slatern44]

If you stick in tool#1 then his atc forward its not going to take you to tool#2 it going to take you to the next tool in the tool changer and the tool changer is at random with it tools. Use MDI put in T1 M06 then T2 and so on when loading your tools so you know for now that you are doing everything correct. And now it sounds like you put 0 on all of your ATC reg so it doesnt know what tool is where.

[panaceabea]

your are correct on the reg for the tool changer, I hi-lighted the pocket column and hit origin and it renumbered them 0-39 and the ability to advance by hitting next tool or atc fwd/rev has returned.

the g54 z is set as 0.00 x and y are the center of my block.

My block is 5.00" above the top of the table.

I started with tool 1 a half inch endmill, gauge length of 4.00"
and tool 2 , a .375 endmill with a gauge length of 3.1701"

Starting with no tools entered in the library I placed a 1/2" endmill in the spindle as tool 1 and touched the top of my block. The z axis machine position is -18.7601 . I pushed the tool measure button and this value was automaticly entered in the geometry column for this tool .

I then hit the next tool button , it placed tool one back in the carousel and I loaded a .375 tool in the spindle as tool 2 . Touched off on the top of the gauge block , machine z axis position reads -19.590 , clicked the tool set button and that value was entered in the H length box for tool two.

the difference in the length of the two tools is .8299" , the same as the difference in the position of the two tools when measured against the gauge block and the numbers entered when I hit the tool length measure button and all seems well.

I now put tool 1 back in the spindle and lowered the tool to the top of the gauge block , machine z position -18.7601 , and set g54 z zero as the top of the gauge block , position readout for g54 z displays 0.00 as exp[ected.

Change to tool 2 and call out z zero , tool moves down to a machine z position of z-18.7601 which would be correct if it were tool 1 . At this point the tool is .8299 above the top of the gauge block and g54 z shows 0.00, if I jog tool two down to the top of the gauge block the machine z shows -19.590 and g54 z shows -.8299

I am sure there is something I am missing here thats pretty simple , but I thought when I called out t2 it should use the offset value for tool 2 but it appears it uses the offset value for tool1 , no matter what tool is loaded in the spindle.

[slatern44]

Type the numbers in by hand and use MDI to move your tools around that way you will see what is going on. Maybe you are not hitting your shortcut keys in the correct order so the controller or you are confused. And turn your machine all the way off and let it sit for a couple of minutes then restart it.

[extanker59]

It doesn't know that you have tool 2 offset in untill you use G43 H2
Maybe? I use a tool setter so I'm guessing but I know that when I use MDI I have to use G43 H___ to get my tools where I want them in Z

[panaceabea]

I assumed it loaded the offset value when I called out the tool change in the mdi like all my other cnc mills, tryed g43 h2 and its still using the offset for tool1 , tryed M6 T202 which my Hurco lathe requires , T2 for tool and 02 for offset =T202 , it loaded tool 2 but still with the oofset value for tool 1 . Also tryed M6 T2 H2 , loads tool 2 , still with offset value for tool one.

Tommorow is a week since its been on the floor, hope I can figure out what i am doing wrong before the first payment LOL

[Vern Smith]

T2 M06
G90 G80 G40 G54
G43 H02
G00 Z0.

This should put tool #2 in the spindle and send the spindle down to the Z offset position you established for G54. Move the table to a position that leaves open space between the spindle and the table (no vises underneath) Type the above into the MDI screen, don't forget the end of block symbols. Set the rapids to 5% and hit GO. Watch the distance to go to be sure it gets to zero before the tool hits the table.

The tool should stop at exactly the height you set your G54 off set from. You can hand jog over to the part and see where you are. To be on the safe side put something in the vise that protrudes several inches above the vise. Set your Z offset for G54 to the top of this piece then do the above.

You must tell the machine what tool length offset to use for tool #2, that is what the H02 does. Tool #3 needs H03, etc., etc.

Vern