Another Tool length Offset Question

robbar10 · Jan 17, 2019

I Bought a used 2000 Hass Mini Mill and I have been trying to set the tool length offsets to no avail.

One way I tried was to take tool 1 and touch a surface. I make that surface g54 z0 and hit the measure tool length offset button giving that tool a 0 offset. I then bring up tool 2 and touch the same surface and hit the measure tool length offset button. a tool length offset goes into the table for tool 2. Then to check I MDI(with tool 2) something like G0 Z.1 but the tool will be nowhere near .1 from surface.

I even go into the tool offset table and add/subtract a few inches from the measured value and it doesn't change the position. It almost seems like its ignoring tool length offsets all together unless it is 0.

I have tried it with the setting for "tool length offset uses work" both on and off according to the procedure for each. Either way seems to not change anything.

Can someone point me in the right direction?

Mike1974 · Jan 17, 2019

When you are calling your tools are you using a G43 or G44 (less common)?

robbar10 · Jan 17, 2019

To call up the next tool I use M06 T2 H02 G43. The height offset that is measured into the table is positive(in this case about 3.2) and is the same as what the position readout shows with that tool in the spindle and the tip touching the G54 surface. The position readout doesn't change even when I add or subtract from the offset in the table.

Hazzert · Jan 17, 2019

Our Haas tool length setting procedure. "tool length offset uses work" is on.

-Touch spindle nose off on height setter 1-2-3 block whatever you use.
-Set this position in a tool length offset (We use G115)
-In MDI call G115 active
-Touch tool off to the same measuring device
-Set tool length offset button

In the tool offset screen the tool length should measure approximately gauge length to tool tip.

Here is the starting code for a tool height call up

Code:

N1G0G17G40G80G90
M31
T1M6( 2 INCH ISCAR FEEDMILL )
T1
( OPERATION 9, ROUGHING )
( WORKGROUP )
( TOOL 1, 2. SHELL ENDMILL )
G54G90G0X-3.675Y2.1438S4000M3
G43Z4.H1M8
Z.1

What happens if you try these steps?

guest · Jan 17, 2019

robbar10 said:
To call up the next tool I use M06 T2 H02 G43.

You need a Z move when you call the offset.

Put tool 2 in the spindle.

Then MDI G0 G43 H02 Z1.0

SeymourDumore · Jan 17, 2019

robbar10 said:
One way I tried was to take tool 1 and touch a surface. I make that surface g54 z0 and hit the measure tool length offset button giving that tool a 0 offset.

OK, that doesn't make sense.
You should not have 0 in the tool length offset....

Anyway, here is a quick one to start with.

First and foremost, set the "T. Offs Uses Work" setting to OFF!

Then: Put a 2" gageblock ( or whatever you feel comfortable with ) on top of the fixed jaw ( or table or... ), jog Tool1 until it touches.
Then: In the offset page with the tool's length offset highlighted, hit "Tool Offset Measure". You should end up with a negative number in the offset register.
Then: Set G54 Z-offset to 0
Then: in MDI type in the following:
T1 M01
G00 G43 H01 D01 ( <- NO NEED FOR A Z POSITION COMMAND ON A HAAS)
G00 Z2.
M00 (<- NEED M00 ON A HAAS, ELSE THE MDI FINISHES, REWINDS AND CANCELS THE TOOL OFFSET )

Now, while you're at the M00, observe the Work Coord position, it should be @ Z2.0, and your tool should also be 2" above the block you've set to.

If all that's OK, then make this test.
Set G54 Z-offset to 2.0

Run the same MDI program again.
Your Work Coord position now still say Z2.0, but your tool should be 4" above the setter.

Let us know if you can replicate the above result.

robbar10 said:
To call up the next tool I use M06 T2 H02 G43. The height offset that is measured into the table is positive(in this case about 3.2) and is the same as what the position readout shows with that tool in the spindle and the tip touching the G54 surface. The position readout doesn't change even when I add or subtract from the offset in the table.

That is because of the Haas implementation of the MDI mode.
When it finishes, it resets the coordinates. You need to stop the MDI and not let it rewind, hence the M00 as shown above.

IWUP · Jan 18, 2019

robbar10 said:
I Bought a used 2000 Hass Mini Mill and I have been trying to set the tool length offsets to no avail.

One way I tried was to take tool 1 and touch a surface. I make that surface g54 z0 and hit the measure tool length offset button giving that tool a 0 offset. I then bring up tool 2 and touch the same surface and hit the measure tool length offset button. a tool length offset goes into the table for tool 2. Then to check I MDI(with tool 2) something like G0 Z.1 but the tool will be nowhere near .1 from surface.

I even go into the tool offset table and add/subtract a few inches from the measured value and it doesn't change the position. It almost seems like its ignoring tool length offsets all together unless it is 0.

I have tried it with the setting for "tool length offset uses work" both on and off according to the procedure for each. Either way seems to not change anything.

Can someone point me in the right direction?

Your tool offset measure value should be the delta from the Z machine zero i.e if you touch your tool off 6" down from machine home when you hit tool offset measure it should say -6.000. Don't change this value to 0. This location will also be your G54 Z0. value assuming you are using that work coordinate
I use one of these for tool touch offs
Pro Touch Off Gage 4- - Edge Technology
If, for example, I touch off on top of my stock using this tool, I have to set my G54 Z value to -4.
For what it's worth I highly recommend this tool, You can run the program in air leaving Z set at zero (4" above your part) to check things before you are ready to go then set G54 Z at -4.

Hope that makes sense

rklopp · Jan 18, 2019

We do something similar to IWUP, but all tools are referenced while the setter gauge is sitting on the machine's table. In our case, we use a 2" setter gauge. Thus, Z=0 for all our tools in the carousel is an imaginary plane 2" above the table. To run a part, we need to enter the distance between Z=0 for the part, which is usually the top of the part, down to this imaginary plane. The distance is the height of the top of the part (or wherever Z=0 is on the part/stock) down to the table less 2.0000 inches. We usually measure the distance using the machine itself (toggling between Hand Jog and MDI/DNC resets the Dist-to-Go values so you can use that as a measuring tool, zeroing the values with any tool touching the 2" setter sitting on the table, else a DTI in T10, then move the setter (or DTI) to the top of the part, touch off, and read Z from Dist-to-Go), but you could measure it with a rule, depth rod on a caliper, or a depth mic. Go to the G54, G55... offset page, and enter using F1 the Z distance you just measured into the table Z column for whichever G5x you are using. Then type -2. Write/Enter, and it will subtract 2.0000". Don't forget the decimal point, or you will only subtract 0.0002".

To summarize, set all tools relative to the table with whatever feeler you like, and Tool Offset Measure each one. Then type in the Z offset in the part offset table based on the distance from part Z=0 (e.g., the top) to tool Z=0, which you will need to measure.

IWUP · Jan 18, 2019

rklopp said:
We do something similar to IWUP, but all tools are referenced while the setter gauge is sitting on the machine's table. In our case, we use a 2" setter gauge. Thus, Z=0 for all our tools in the carousel is an imaginary plane 2" above the table. To run a part, we need to enter the distance between Z=0 for the part, which is usually the top of the part, down to this imaginary plane. The distance is the height of the top of the part (or wherever Z=0 is on the part/stock) down to the table less 2.0000 inches. We usually measure the distance using the machine itself (toggling between Hand Jog and MDI/DNC resets the Dist-to-Go values so you can use that as a measuring tool, zeroing the values with any tool touching the 2" setter sitting on the table, else a DTI in T10, then move the setter (or DTI) to the top of the part, touch off, and read Z from Dist-to-Go), but you could measure it with a rule, depth rod on a caliper, or a depth mic. Go to the G54, G55... offset page, and enter using F1 the Z distance you just measured into the table Z column for whichever G5x you are using. Then type -2. Write/Enter, and it will subtract 2.0000". Don't forget the decimal point, or you will only subtract 0.0002".

To summarize, set all tools relative to the table with whatever feeler you like, and Tool Offset Measure each one. Then type in the Z offset in the part offset table based on the distance from part Z=0 (e.g., the top) to tool Z=0, which you will need to measure.

Personally I like to use the back of the vise to touch off my tools with the 4" Edge Tech gauge then use a 2-3-4 block and a Haimer to measure the distance from the touch off point to top of my parallels. That way I'm not reliant on any variations in the stock thickness. Depends on the job though, sometimes on a few pieces going off the stock top is fine. Most of the time I'm more concerned about tolerances than the end user.

robbar10 · Jan 18, 2019

Thank you all for taking the time to respond. I was not aware at the MDI rewinds.

I used seymourdumore's method and it worked. I was able to set 2 more tools and have them both measure and go to the right height.

Now My problem is that I don't understand why it works. With "tool Offset uses work" off, is the WC offset the difference in distance from the tool touch off point and the work coordinate system? For example a 2" gauge block on top of the part to measure tools and the part below it the offset would be -2.0"?

In this case also does that make the tool length offset a measure of how far the tool tip is from machine home(or the tool change height in my case)? Could use still premeasure tools outside the machine using this method?

SeymourDumore · Jan 18, 2019

robbar10 said:
Now My problem is that I don't understand why it works. With "tool Offset uses work" off, is the WC offset the difference in distance from the tool touch off point and the work coordinate system? For example a 2" gauge block on top of the part to measure tools and the part below it the offset would be -2.0"?

Yupp, You've got it! That is exactly how it works.
By having that setting OFF, you're indicating that the tool length in independent of any active work coordinates, and the length offset is simply the distance from Z-home to the reference block.
Then, by entering a negative or positive value in the coordinate offset ( G54 or any other ), then you're telling the machine that the work is that far above or below the reference block.

As far as setting it outside of the machine, yes, you can just make the appropriate changes in your tool setter.

Frankly tho, I don't see much value in a pre-setter, never have.

Search

Largest Manufacturing Technology Community on the Web

Search

Another Tool length Offset Question

robbar10

Plastic

Mike1974

Diamond

robbar10

Plastic

Hazzert

Stainless

guest

Guest

SeymourDumore

Diamond

IWUP

Aluminum

rklopp

Diamond

IWUP

Aluminum

robbar10

Plastic

SeymourDumore

Diamond

Similar threads