TOOL PRESETTING ???

[MACHINEMASTERG]

just wondering??? we have always touched our tools off in the haas to the top of part or fixture and set the toollenth offset leaving the work off set at z0 ..with the presetter it measures the tool from gage line to tip how would that be set up in the haas for workoffset z0???how do you set z0

thanks for all replies

[Jack K]

I touch off the spindle with a 8 inch standard to the workpiece and then add the 8 inches to the offset I get. My Z offset number is a positive rather than a negative number.

 

Presetters are the way to go!

 

jack

[Guest CNC Apps Guy 1]

Our tool offsets are the gage length of the tools (Gage line to tip of tool with a positive value) and fixture offsets are wherever they are in space with values in all three (sometimes four) axes. Presetting is THE way to go. That way whatever condition the material is in I can always touch off a tool and still have the right length as opposed to touching off the top of the part that may have been milled away.

 

JM2C

[MACHINEMASTERG]

thanks for the replies... but can you explain a little more on how z0 is set i understand you measure all tools from gage line to tip then input that value into tloffset page in positive value then what sets the z0 to fixture or part ????

[Marty A]

well where ever are zo is at on

our detail that will be are zo.

we will set are machine from the spindle

using a 4 inch indicator gage block.

if zo is the bottom then we don't add

anything.let's say zo of the detail is 1.0

inches up, then we would subtract the 1 in and that would be our zo.

 

marty

[Jack K]

"Z" 0 is your fixture offset, spindle face to workpiece. The cool thing about presetters are once your tool in in the toolchager it is set no matter what workpiece you are running. Just like my favorite informercial "Set it and forget it"!

 

jack

[MACHINEMASTERG]

ok jack let me see if i got you... measure tools put that number in tloffset page positve number ..take a master tool that you have set to 8.00 gage line to tip and touch off top of part or fixture top ..then that number minus the 8.00 tool lenth that goes into your g54 or g55 what ever workoffset you are using and this will be a negitve number then all tools from then on out just measure in the presetter and put in tlooffset page ?????thanks for all responces i think we are going to go this way just tring to get a better understanding on this weve never worked this way...

[Jack K]

I take add my 8 inch standard to whatever number I touch Z at. Example if I touch my spindle face between my standard and the work piece and have a number of 20.5... I add 8 inches to that. That would make my G54 Z offset a negative number. By the I am useing a Fanuc 18M I asume it would be the same for all.

 

jack

[MACHINEMASTERG]

so then from the spindal face to the work would be g54 x0 y0 Z-28.5 and by having the tloffset # set to positve numbers it would stay short of the g54 z0 buy the number in the tloffset page ...i think i see said the blind man thanks for all help >>>>

[jspangler]

Hi

COOL. I had been wondering about a better way to do this for a while now.

 

thanks

 

John

[Chris Rizzo]

Here's what I do for my Haas-

 

-I set all tools to the table using a .500 gage pin in a go/no-go fashion.

-Then hit "tool offset measure"

-Then -.500, enter.

 

For my material g54-g59, I slap a height gage right on the table and measure my stock height...up from the table. Enter that value for my g54 Z offset.

No matter what part I am cutting and what fixture offset (g54-59), all the tools are set the same. Allows to slap fixtures in and out, and don't have to re-set the tools every offset change...

m2c

[LNDCAD]

What a GREAT forum! I just had this topic come up in a CNC class I teach. I always touched tools off the workpiece for class work, but wanted to show them how it is done in the "real world". You guys answered my question before I even got a chance to ask it. How did you do that ??? THANKS!

[Guest CNC Apps Guy 1]

The nice thing about setting the tools from a common location is that it's independant of the part, which IMHO is as it should be. I shoudl not have to have a workpiece in the machine to touch off my tools. This opens the door for material variance and a host of other anomalies that can and do occurr on occasion.

 

HTH

[crazy^millman]

Well the Mazak Mills and the Thermwood with a touch setter do this task the way same way. You touch off all the tools with the touch setter you then touch off one tool to set the Z postion in your workoffset and hit the green button and go. The cool thing about it is change a tool or what ever and rerun the automatic tool touch off cycle and when done hit the green button off you go simple as that.

[Bob_Looney]

I changed the Z zero for my cnc to be the tip of a standard tool (tooling ball in holder) to the inner ground surface of my vise. I can then set the G54 position to a known Z value based on parallels or fixture thickness for a given part, no measuring or touch off required.

Tooling offsets are the difference between the std tool and my cutting tools. I then use G10 to load the G54 offsets from the program to the control.

[specv]

This is the way we used to do it before we had probes, 1st: take a 1" travel indicator put it in a collet 2nd: put it in the presetter and hold it at zero get a gage length from the presetter

3rd: take the indicator and touch the workpiece until it reads zero 4th: take the machine position value (it should be a negative number) and subtract the gage length of the indicator setup so you have the distance from the spindle nose to the workpiece.

[MACHINEMASTERG]

thanks for all the replies we just got our new presetter and we are switcing to the new system seems better already ..if you always do what always did then you will always get what you always got ...onward and upward !!!!!

[maestro]

The true definition of insanity:

 

Doing the same thing the same way every time and expecting a different result.

 

How many of you have worked for someone like this?

[Hacsta]

man this place is great!!!!

MMG, WAY TO GO!!!

can't wait to set the machine up using the new tool setter

[Hardmill]

Our presetter has a macro built into it to add

the length of the gage tool to the offset (so all

offsets are pos). Touch your gage tool only off

the workpiece and "viola" your done.

It a thing of beauty.

 

"If you have the resources I highly recommend

picking one up" Ferris Beuller

 

PEACE