Need some help with offsets using auto tool setter

My current Haas mini mill does not have a tool setter or probe.

I am manually checking both my tool lengths and my stock offsets off my table height on the machine, and that has always worked well for me.

I recently purchased a Haas DM-2 ( Pre- NG controller ) that does have a wireless probe and tool setter, so my plan was to stick with my normal measuring whereby everything is measured off the table height.

This is a used machine, so the previous owner had the measuring set up different than what I am use to.

I thought it would make sense to stick with a consistent way of measuring both the tools and the stock to avoid mistakes in my CAM workflow

in doing some testing it looks like the figure that I need to deduct from my measurement from the tool setter is -20.8891

So here would be an example of measuring 1/4 flat end mill with my tool setter

The tool setter measures the tool at a length of 3.7373
3.7373 Minus 20.8891 gives me the 17.1518" which is the measurement from my table to the bottom of the end mill.

For now, I will make that adjustment each time after measuring the tool, but it would sure be nice to have that adjustment calculated automatically.

So my question is: what code would I need to add / change on my probing in order for this to adjust this automatically?

If there is another way to accomplish this I'm open to any suggestions...

Thanks,

Kent

Measuring tools in one machine, and putting them in another isn't such a hot idea to me.
Usually, machines with Tool Setters measure from the table up, which is why the offsets are positive. Trying to convert this to "bottom down" and then put in another machine is a little scary to me.

DouglasJRizzo said:

Measuring tools in one machine, and putting them in another isn't such a hot idea to me.
Usually, machines with Tool Setters measure from the table up, which is why the offsets are positive. Trying to convert this to "bottom down" and then put in another machine is a little scary to me.

Click to expand...

The reference for all settings in machines with probes and tool setters is spindle face, which represents tool length 0. Therefore the length of all tools loaded in spindle (including the probe)have positive value, value which represents their physical length. The Z position of the tool setter's face is defined in machine coordinates, and is set simply by touching it by spindle's face or by tool of known length.
This approach can of course be implemented also for manual touching off the tools.

Stefan

Here's the list of Haas Tool Offset macro variable numbers:

https://www.haascnc.com/content/dam/haascnc/videos/bonus-content/ToolOffset.Macro.Vars.pdf

Length geometry starts at #2001 for T1 and goes up to #2200 for T200.

To answer your question directly, you might use something like the following statement somewhere in your code:


That said, if you're going to regularly use your 2nd machine as an offline toolsetter, you may has well keep things consistent and just use the positive number measured straight from the second machine (actual length from the gage line). You'll spend a bit of time remeasuring all your tools and tweaking your Z-axis work offsets in the first machine, but long term it'll help prevent errors that would easily result in a collision.

Orange Vise said:

Here's the list of Haas Tool Offset macro variable numbers:

https://www.haascnc.com/content/dam/haascnc/videos/bonus-content/ToolOffset.Macro.Vars.pdf

Length geometry starts at #2001 for T1 and goes up to #2200 for T200.

To answer your question directly, you might use something like the following statement somewhere in your code:

Code:

#2001 = #2001 - 20.8891

Click to expand...

Hello Orange Vise,
What you're suggesting would not work at all. In your example, 20.8891 is being subtracted from a value that is registered in a Tool Length Offset, when what needs to occur is to plug a value into the Tool Length Offset.

As explained by Probe, it's usual for the Spindle Gauge Line (Spindle Face) to be the Reference Tool Length that has a Zero Value. Accordingly, it's Machine Coordinate Value will be the greatest minus value when it is touched off on the Tool Setter. This Value would be stored in a Common, Non Volatile Macro Variable for use in calculating the Tool Length Offset for all other tools. For example, the Machine Coordinate value of -20.8891 may be stored in Variable #550.

To get the Offset Number to set, the Tool Number will either be passed to the Macro as an argument, or retrieved by reading the System Variable for the current spindle tool or the lasts last "T" code command from System Variable #4120 and would look something like the following.

#[2000 + #4120] = #5063 - #550

In the above example using the following values:

#4120 = 4

#550 = -20.8891 (Stored Reference Machine Coordinate Value)

#5063 = -15.2342 (Current Z Skip Signal Position Value when the Tool being measured touches off on the Probe)

then Tool Length Offset 4 (#2004) would receive the calculated value of 5.6549.

Regards,

Bill

Hello,

I might not have explained myself well..... I will continue to measure on my other machine manually with a gauge like I have in the past.

Thanks,

Kent

PROBE said:

The reference for all settings in machines with probes and tool setters is spindle face, which represents tool length 0. Therefore the length of all tools loaded in spindle (including the probe)have positive value, value which represents their physical length. The Z position of the tool setter's face is defined in machine coordinates, and is set simply by touching it by spindle's face or by tool of known length.
This approach can of course be implemented also for manual touching off the tools.

Stefan

Click to expand...

Yes. Correct.
But shuttling between machines and mathematically trying to "adjust" is still, not confidence inspiring to me. I wouldn't.

Thanks Bill...

I think this may be my answer....

I may have to come back with a few questions once I digest this a bit..

Thanks again...

Kent

DouglasJRizzo said:

Yes. Correct.
But shuttling between machines and mathematically trying to "adjust" is still, not confidence inspiring to me. I wouldn't.

Click to expand...

Hello Douglas,
The only difference would be the tolerance of the Gauge Line of the spindle, normally quite small; particularly with machines of like manufacture. It would really be no difference than using an external Tool Setting device. Provided that all tools for the second machine where measured by the one machine, then setting the Z Work-shift of the second machine would sort out any minuscule difference in the Spindle Gauge lines.

Regards,

Bill

Just to clarify, I am only going to be using the tool setter for measuring tools on the DM-2 machine for that machine only,

I will continue to measure the tools manually on the mini mill like I have in the past.

What I originally meant was that I am use to measuring everything ( tools and work piece ) off the table height, so I was hoping to keep doing it that way just out of habit.

kentd said:

Just to clarify, I am only going to be using the tool setter for measuring tools on the DM-2 machine for that machine only,

I will continue to measure the tools manually on the mini mill like I have in the past.

What I originally meant was that I am use to measuring everything ( tools and work piece ) off the table height, so I was hoping to keep doing it that way just out of habit.

Click to expand...

Hello kentd,
What do your mean by "off the table height"? Are you using the face of the table as the reference plane? Even when setting the Tool Length Offsets manually, without an integrated Tool Setting device, it's relatively simple to implement a Tool Measuring Macro, using one of the many, off the self, dial indicator type, manual Tool Setting Devices.

1. Get a "Z" Machine Coordinate value for the face of the Spindle to the Tool Setting device when the dial indicator reads Zero and store this value in a Common, Nonvolatile variable that's not used elsewhere.

2. Execute the Tool Length Measure Macro Call Block to pass the Tool Number of the Tool to be measured to the Macro and have it loaded into the Spindle.

3.Manually bring the Tool to be measured down to touch off on the Manual Tool Setter and when the dial indicator reads Zero, run the remainder of the Tool Measuring Program to calculate and register the Tool Length Offset.

The program will look something like the following.

M111 T06 (Macro Call Block using a Custom M Code to call the Tool Length Measure Macro)

%
O9001
N1 G91 G28 Z0.0
T#20 M06
M00
(MANUALLY MOVE TOOL TO TOUCH OFF ON TOOL SETTER)
(ONCE THERE SELECT AUTO MODE AGAIN TO RUN REST OF PROGRAM)
#[2000 + #20] = #5023 - #550
G04 X0.100
G91 G28 Z0.0
M30
%

Regards,

Bill

DouglasJRizzo said:

Yes. Correct.
But shuttling between machines and mathematically trying to "adjust" is still, not confidence inspiring to me. I wouldn't.

Click to expand...

Agree 100 % !!!
Stefan

Hi Bill,

Yes you are correct, when I said "off the table height" I meant the face of the table as the reference plane.

Thank you very much for your sample code you put together....

One other quick question...

I was trying to find the actual program code that gets called up on the machine during a tool measurement, and I can't seem to find it. ( I wanted to copy it onto a thumb drive )

I couldn't seem to find it in the list of programs in the memory section.

Thanks,

Kent