Touching off the stock and setting the tool height and z

[AlexDobbie]

I have just got access to a HAAS Mini Mill, I have been through the training that the installer went through but I am having difficulty relating the tool length to the z of the machine ( I can set a work and tool offset and run a program) ?

I was shown to touch off the top of the stock and set the tool length to that with the z co-ordinate being zero. This works fine for some stuff but it is a bit of a pain setting the same tools up again and again ( we do alot of surfacing with the same 3 tools )

How does the z-0 of the work offset and the tool offest relate ? Is it something that I can do or do I need to get the techs back again ?

[-Chris-]

Hi, i have two vf 4s i setup and run daily. We set all tool lengths to the same place, on the 2 inch edge of a 123 block on the table of the mill. Then i will set up my fixture offset by first squareing my vice and setting a stop of some sort. i use a 123 block in the vice jaws and use my edge finder for X & Y ZERO.Now to find z zero i dont use the top of stock but a value set from the top of the parallels my part set on. So i bring say tool 1 in to the spindle and i jog it down to the top of the 123 block plus a .250 gage block (so we've got 1inch plus .25 gage block)on top of my parallels.Then you push offset button and go to the tool length page and look at tool 1 length value type that into a calculator now look to bottom left on the screen and youll see a current z position subtract that value from t1 tool length and then go to your fixture offset say g54 x---y---z and type in that figureand hit f1 to set thet value. i then type-1.25 hit write enter and the value is now set to the top of the parallels so now say our part is 2.5 inches thick i type 2.5 hit write enter and the setting is adjusted up to the exact top 2.5 above parallels. it seems like alot to go through but its really not and its easy to change a dull or broken tool if you set all lengths to the table and i can set up 5 vices and fixtures offsets with a 123 block and my gage block

[Pondo]

This is what I do in my Minimill:
1-Pick something to set all of your tools to. I have a vice in my machine that hardly ever gets removed, so I use the top of the vice about 1" behind the fixed jaw. You can use the table, but in a Minimill it's kinda hard to find a spot to reach it. Any fixed flat surface will work.

2-Set your tool lengths to the top of the vice or whatever. I use a .500 gage block to set the tools. Handwheel the tool to below the top of the block and in .01/click, move the tool up one click at a time till the block slides under it. Move block out of the way, then move the tool down one click. Switch to .001/click and raise the tool one click at a time until the block slides under again. Move block out of the way, then move the tool down one click. Switch to .0001/click and raise the tool one click at a time until the block slides under again. Highlight the correct tool length offset for the tool and press Tool Offset Measure (right under F1). This puts the current machine position in the offset. Since I use a .500 block, I then type in -.500 and hit enter to adjust for the gage block. This way all my tools are touched off to the same exact Z level.
The reason for moving the tools up until the block slides under Vs. down onto shim stock or something is to avoid breaking the corners off of carbide tools. HSS may be able to take it, but carbide will crack.
Plus it's dead on balls accurate and repeatable.

3-Set your Z offset in G54 or G55 or whatever. G54 Z offset will be the distance from the surface you touched off your tools to wherever on your part you want it. The top of the block for example. Use an indicator to find the distance or use a tool. For example, I know it's -1.493 from the point I touch off my tools to the ways of the vice. If I use 1.5" parallels and have a 2" part, I know the Z offset is 2.007. If I need to measure it or set the Z offset exactly, I use an indicator in the spindle. Handwheel the indicator to read 0 on the touchoff surface. Press "POSITION" twice, then page down once to get to the operator position page. If Z is blinking, just press "ORIGIN" to zero it out. If it's not, either press the Z axis select key or type Z and hit ORIGIN. Move it to where you want the Z set and then down until it reads 0 again. The Z reading on the display is the distance from the touchoff surface to the surface you are setting as Z0 on your part. Set that # as the G54 Z offset.

Once tools are touched off to the same point they can be used on every part since the G54 Z offset is always the distance from that surface. It can be + if the work is taller or - if the Z0 is below the touchoff surface.

I also have 2 VF-4's with pallet changers on both. I took steel blocks and bolted them to a corner of each of the tables. I faced them to the exact same location from the machine 0. I can then touch off a tool to one of the blocks and use that tool and offset on either pallet in either machine.

[lkenney]

An easier way for a new user to set his tooling but closely related to the processes already written about.

We use a mechanical Offset gage that is a 2" block with a 0.0005" indicator built into it. (The Blue Block) to get a more constant tooling zero than we do with touch off blocks because many people do not have the same feel when using a sliding gage block usually 0.25, some people use a 123 block the same way. These Indicator gage blocks run about $75.00 to $125.00 and will save you much more than in broken endmills, and destroyed material. From job to job and shift to shift we use these little gage blocks to set the zero consistantly. They also make electronic ones but we have not bought those yet. We set these gages on one corner of the vise and set every tool that goes into the tool changer -ALWAYS-.

Running under manual control MIDI at about "1000" RPM, Our MIDI Line reads S1000 M03 ( speed 1000 rpm Clock Wise rotation) We then use an end mill to touch off on the material at a point that will be cut away by easing the end mill down to the stock and just barely touching off, should be just a hair ring showing. Us the "handle jog" set on the 100 resolution 1/1000 per step. hit "reset" and stop the machine at this point. Leave the Z axis touching the material.

Then we go into the "Offset" screen locate the tool that we are using. I almost always have 1/2" end mill in the No 6 tool slot and usually use this end mill to set from. I would then go to the offset screen, locate Tool 6 and at the bottom of the screen will be a lin showing your current tool location.

Compare the two settings if the BOTTOM (Material) Z ZERO is LARGER than the tool zero subtract the tool zero from the material zero (material zero line shows -11.456 -- Tool 6 is zeroed at -10.024) 11.456 - 10.024 = -1.432

If the BOTTOM (Material) Zero is SMALLER than the Tool Zero subtract the Material Zero from the Tool zero. (forget about the negative numbers) you are just looking for the distance between on zero and the other. Working in positive numbers is easier for most people. In this case your material zero is higher than the gage block so your offset will be a positive number.

Push the "Up Page" key and the material Offset page will show up starting with #52. (at this point don't change G52) G54 is the first offset that you can use. put your curser bar on the G54 (or other) Z offset line and key in the result of the above calculation then press "F1" to replace the Z Value there with the new Z value you calculated. Now all your tools are zeroed for that material. Set you "Y" and "X" offset values. (We usually use the Left rear front corner of the rear jaw of the vise or if there is a material overhang the left rear point of the material.) Make sure you know where the material sits in regard to the machine. with material stops or gauging points so you can locate the following material in the same location.

If you break or need to change a tool, just zero the new tool with the Indicator block and you are good to go.

Hope this helps

Lowell