Tool Height Offsets

[JamesBond]

I am curious how other people set up their tools and part offsets.
I'm sure if you ask 10 people you will get 10 different answers.
I'll describe the steps I do when I set up my tools and a part surface.
The method I use works, but I'm sure other people might have an easier method.

Background:
I use an electronic XYZ edge finder for locating the part,
and a 2" electronic Height block for setting up each tool's offset.
If I'm using a vise, I'll use the rear surface as my reference.
I always keep T1 as my XYZ edge finder.

Set T1 (done only once)
1. Touch T1 (XYZ edge finder) to my reference surface,
and zero the tool. (without the 2" height gauge)
2. I add 2.0" to T1's offset.

Set each tool:
3. Using the height block, Zero each tool to my vise.

Setup for part surface:
4. Using T1 (XYZ edge finder) touch the top of the part.
5. Add T1's tool offset value to Z height.

These steps have worked well for me.
I explained what I was doing to a friend and he had a very puzzled look,
so I'll guess other people don't do it quite the same way.
The one thing I don't like is if I forget step 5.....Crash!@%$#
I would like to hear how other people do this.
-JamesBond

[hardmill]

As you said 10 people will have ten opinions.
I Always try to set all my tools off the top of
the part(just my preference). If what you do
works for you stay w/ it just don't forget step5.
The least amount of steps in my opinion always
makes the most sense.

By the way Welcome to the forum .
You'll find lots of helpful advise here.
Good to have you aboard.

[CAMmando]

5. Add T1's tool offset value to Z height.

Depending on what type of control you have, there may be a parameter that you can store the gage length of your t1 in. Check your manuals.

On toolroom type cncs I set the tool right to the Z=0 and go.

Here are 2 Methods I have used for production machines.

Our machines have Probes (work setters) and Tool setting blocks.

The controls have two parameters that are set once (unless some adjustment to the machine is made they can be reset).

1. A value that represents the distance from the spindle gage line to the top of the tool setting block when the block is seitting on the table.

2. A value that represents the distance from the gage line to the tip of the probe. (similar to the length of your tool 1).

Our machines have 30 tool changers. We normally leave t30 empty because often t1 winds up being a large face mill. If the face mill is too big, it will hit the adjacent tool in the tool changer when it swaps out. Anyway, we have T29 As our probe and T28 as a drill chuck for indicating or edgefinders.

To set up a job,

1. We set the tool length by touching off on the tool setting block (the control will read the position when contact is made or you could enter the Z value in manually)

2. We touch our Z=0 surface (usually it is top of part as hard mill said)

The machine has all the information it needs.


I am going to be changing shortly to presetting tool lengths outside the machine. A fancy optical presetter is not in the budget so ... either we buy a mechanical presetting station or make one. I made one at another shop as follows:

Again this is for production environments when you cant afford an expensive tool presetter but want to set tool lengths off line, you can do the following (assuming your control has the parameter for tool setting gage height or some equivelent ).

INITIAL SET UP - ONE TIME ONLY:

-Make a "Standard", Use a piece of 1/4" Hardened Drill Rod With one end ground square. Mount the rod in a dedicated tool holder (endmill holder is fine and a tack wekd for good measure doesnt hurt either to make sure the rod doesnt move.)

-Make a Tool setting station, using a ground steel plate with block mounted to it with a tapered bore that matches the taper of your spindle (CAT 40 or whatever).

-Put the standard in the machine and touch it off to a reference surface. Record the value.

-Put the probe or XYZ edgefinder in the machine and touch it to the reference surface. Record the value.

-Subtract the numbers and enter this value in the parameter your control uses for work setter or tool setter height compensation.(you need to check the manual to see what parameter you have and what the value represents.)

NOw that the hard parts over to set jobs up:

-Using the presetting station and a height gage, place the "Standard" in the taper on the presetting station. Zero the height gage on the tip of the rod.

1. Put your tool/tool holder in the presetter and measure its height (you are measuring the difference between the standard and the tool) Record on toolsheet or tag. There are nice re-usable plastic tags that you can buy from MSC that can be written on with marker and re-used. They fit around the flange of the tool holder.

-Repeat for all the tools.
(Remember the machine is running another job while you do this UPTIME = $)

2. When you set your Z work offset you just touch off on Z=0 with your XYZ Edgefinder or probe.

3. Enter all the tool Length offsets.

Hope this is helpful or at least interesting cuz' Im tired and its waaayyy past my bed time.

BTW Welcome to the forum (Im pretty new here myself)

Dave

[hardmill]

Originally posted by CAMmando Depending on what type of control you have, there may be a parameter that you can store the gage length of your t1 in. Check your manuals.

Golf clap "CAM"
Missed that one
PEACE

[HuFlungDung]

Originally posted by hardmill As you said 10 people will have ten opinions. I Always try to set all my tools off the top of the part(just my preference). snip

Hi James, and welcome, you special referral, you

This guy helped me a ton with writing scripts for Bobcad, back when I was heavy into that.

I do what Hardmill does. I have also thought of switching over to a slightly different system, but my old programs keep me going back to the old system. Plus, I use a heck of a lot of different tools (drills, taps and reamers) that mean I have to change tools in a given station anyway

I would always use the top of the part as the Z datum.

The new system I was contemplating was dedicating a single work offset (such as G54) as the "master reference" plane. Then, I would dedicate one toolholder as master, and set all other tool lengths relative to this master. Then, when setting up a new job, I would only check the Z datum with the master tool, and adjust the G54 offset accordingly. Then, I would not have to touch the rest of the tools.

I actually purchased a Fowler digital height gauge for setting up my tools relative to the master, but I haven't yet found a corner of my crowded shop where I can park it and leave it be.

[JamesBond]

Thanks for the responses.

I forgot to mention, when I set up my part, I am using G54.
After HuFlungDung mentioned it, I realized not everyone uses G54.
(I don't think I could live with out a G54.)
I like using something other than the part to set the tools,
that way the tools can be loaded ahead of time and separate from the part.

I am using a Haas controller, I dusted off the manual and looked
to see if there was some sort of setting to add in the a tool offset.
So far the only setting that might help, is one for setting the tool offsets
so the machine will use either "relative to the current work coordinate Z offset" , or "offset equals the Z machine position"

-JamesBond

[HuFlungDung]

The way my Shadow controllers work, is that you can work outside of all work coordinate offset systems if you want to. G54 is the first of 6 available work offsets. G53 cancels any work coordinate offset in effect.

I am not sure if the FANUC clones work that way or are you automatically in the G54 coordinate offset by default? I need to prepare about learning FANUC style, in case I upgrade machinery one day. So far, I am using FANUC controller clones in lathe only, so I don't get to practise much with the aspects that pertain to mills.