My method of tool length measurement

[badbascom]

So on our Fadal VMC we find X0Y0 with either a edge finder that sends a signal to the controller or locate a hole with an indicator and assign to a fixture offset #, we leave Z alone and zero each tool on the applicable fixture using a piece of paper. The one time I zeroed Z on the fixture offset I almost sent the tool thru the machine table.

 

So Im assuming my method is very antiquated, what is the best practice and technology I could add (probes, etc) to set-up fixtures.

[kh012]

on our fadals we use the utility cycle or the SL, command to touch off the tools on -Z- to wherever -Z0- is in the program.

this puts the tool length into the geomety page not the fixture offset.

our fixture -Z- values are only to set the differance in hieght between the first fixture and the second fixture etc. we also use this value to do a globle adjustment

of all the tools that run on that fixture.

 

Ken,

[badbascom]

on our fadals we use the utility cycle or the SL, command to touch off the tools on -Z- to wherever -Z0- is in the program.

this puts the tool length into the geomety page not the fixture offset.

our fixture -Z- values are only to set the differance in hieght between the first fixture and the second fixture etc. we also use this value to do a globle adjustment

of all the tools that run on that fixture.

 

Ken,

 

Thanks, do you zero tools with paper shim or some better method?

[Guest CNC Apps Guy 1]

The BEST method when using Z- length offsets (which I detest in the first place but that's a story for another day) is to get a tool length setter (see below) and put that tool setter on the table or some other location that won't change.

 

Then in your work offset you have the distance from the setter to your part Z zero. This is superior to the paper/shim method because once you remove material from the initial setting position, you can;t ever go back and reset something.

 

If that's not a possibility, I prefer a gage pin over paper or shims.

 

JM2C

[badbascom]

The BEST method when using Z- length offsets (which I detest in the first place but that's a story for another day) is to get a tool length setter (see below) and put that tool setter on the table or some other location that won't change.

 

Then in your work offset you have the distance from the setter to your part Z zero. This is superior to the paper/shim method because once you remove material from the initial setting position, you can;t ever go back and reset something.

 

If that's not a possibility, I prefer a gage pin over paper or shims.

 

JM2C

 

Thanks, please give me the other story, pretend its tomorrow haha. Are Z-length offsets not the best way. I only do it the way I do because I dont know any better.

[kh012]

we use tool lenght setters or shims/gage blocks which ever is conveniant. if you use the utility cycle you tell it the hieght of

your block/shim. you can also add in the differance to Z0. the cycle will do all the calculations to set the tool length. if you

are running 21 tools on 20 fixture locations and you need to change a tool then you only have to retouch off on the first fixture.

all your -Z- fixture offsets remain unchanged. also helps if your holder/tool length changes.

 

HTH Ken,

[Guest CNC Apps Guy 1]

Personally I like Z+ Tool Offsets because I can preset them offline, and I can use the same tool across multiple fixtures without having to scratch my head and wonder where my offset is coming from. ALso, if you ever migrate to HMC's or 5-Axis, you definitely do not want to be using Z- offsets.

[Rockness Allen Machine]

Personally I like Z+ Tool Offsets because I can preset them offline, and I can use the same tool across multiple fixtures without having to scratch my head and wonder where my offset is coming from. ALso, if you ever migrate to HMC's or 5-Axis, you definitely do not want to be using Z- offsets.

 

Please explain the Z+ offsets. On our verticals we use Z- offsets across multiple fixtures and pallets with a standard offset block. Next year we plan on geting a horizontal and would like to hear how you use a Z+ offset.

[YoDoug®]

Z+ TLO is like in the picture below. Your tool offsets are positive measure from tool tip to spindle gauge line. Then your work offset is your spindle guage line at Z0 off your part program.

[BenK]

The way I used to do it was to have a post off in the corner of the table that is about 6" to 8" tall. All of my tools would be touched off of the post using a .5" dowel pin. Than my fixture offset was the distance between the top of the post and my part zero.

[Guest CNC Apps Guy 1]

If you plan on using a laser or touch style breakage system you'll have a tougher time using Z- offsets too.

[Charlie Pierson]

I'm w/ Doug.

 

Another benefit of the TLO being the actual length of the tool (gage line to tool tip) is that the tool is now transportable between similar shank machine tools even if you have to swap a pull stud to go from , say, a Mazak Cat40 to a Kitamura Cat 40.

 

my .02