Tool offset (Haas control question)

I set my tool offsets 4" above my vise then subtract that measurement from my part top like many people do. Up to now, I do the math on a calculator then input the sum into the control. On occasion I'll make a mistake with the math or inputting it into the control so I'm constantly checking and rechecking myself which takes up time. Since the offset distance remains the same (unless I break the probe tip on my Haimer 3D Taster) is there a place in the Haas control I can input my off-set measurement so I can just touch off the part top and let the control subtract the offset and insert the sum into into my z work coordinates?

You could put a -4.000 in your work offset z.

Sent from my SM-G900R4 using Tapatalk

That does not answer the question.

Quote:

---

Originally Posted by l u k e

That does not answer the question.

---

Try it

4 inches is from the top of the vise not the top of the part, what you suggest makes no sense.

I posted in this thread LINK for use on a Fanuc control

see if it is of use

Well, short answer is, unless you drastically alter the method by which you set the tools, you'll pretty much always be limited to typing in a compensation into the work offset Z-value. In order to NOT type anything in, the machine has to know more information since simply pressing the "tool offset measure" or "part zero set" buttons are strictly for obtaining machine coordinates, but you need more than that.

There's lots of ways to make the machine do the math for you, but they all pretty much require you to measure that height difference then type it in somewhere. Having said that, whenever I find the height difference in situations like this, I use the "operator" position screen to do it rather than typing anything outside of the machine. You can manipulate the "operator" position values (Z in this case) to measure the height change for whatever you want within the work envelope, then type that number and set it as your work offset Z-value. However the machine will NOT input the value for you, it simply displays it for your reference, then you type it in.

Okay so the looooonger answer is that you could accomplish your goal of not typing anything into the machine, but it would require your TLO values to be stored as gauge heights (positive value distance from the bottom of the tool up to a reference plane on the spindle). When using gauge height, the work offset Z-value represents the machine coordinate distance to <<bring the spindle reference plane down to the workpiece origin>> (-19.0000" or something). Then, this distance is compounded by the TLO values which are stored as positive numbers (3.5000" or something). The end result is the same thing as you have now, but the measurements traditionally serve different goals....your current method is quicker and easier to understand; the gauge height method is a little more process-friendly however requires deep understanding of the active offsets within the machine. There are many ways to botch the gauge height process, most of which will result in you annihilating the toolholder and/or workholding.

All things being equal I think the gauge height method would be more cumbersome because you would need to find a way to qualify the physical height of the tool which is a departure from your current method. Some places do it offline using a calibrated fixture, some places do it inside the machine using a big block of known height (and type some stuff). But either way it would probably not help your process right now, just complicate it.

At least, IMHO...

The short answer to your question is no.

Quote:

---

Originally Posted by l u k e

I set my tool offsets 4" above my vise then subtract that measurement from my part top like many people do. Up to now, I do the math on a calculator then input the sum into the control. On occasion I'll make a mistake with the math or inputting it into the control so I'm constantly checking and rechecking myself which takes up time. Since the offset distance remains the same (unless I break the probe tip on my Haimer 3D Taster) is there a place in the Haas control I can input my off-set measurement so I can just touch off the part top and let the control subtract the offset and insert the sum into into my z work coordinates?

---

Quote:

---

Originally Posted by kla64

You could put a -4.000 in your work offset z.

---

Quote:

---

Originally Posted by l u k e

4 inches is from the top of the vise not the top of the part, what you suggest makes no sense.

---

If your offset distance remains the same, then shouldn't you be able to subtract that value from your Z offset instead of the -4.0" as suggested? Basically letting the machine do the math instead of a hand calculator.

Ynda is getting where I'm coming from, so just to clarity for the others that suggested I just put -4.0 in Z.

This is my current setup.
http://i550.photobucket.com/albums/i...pspiutv6hx.jpg

The the difference between my zero point on the touch-off gage and the zero point on my 3D taster is 7.8195" this is my constant off set value.

So what I do is subtract 7.8195 for the part top measurement and input a (-) value if the part top is below the touch-off gage and a (+) value if it's above.

It was suggested that I just put a -4" value into the control and touch off. If I put my off-set value of 7.8195 (+ or -) into my control, then touch off the part top, the control changes the Z value to -7.1158. On this particular part the final value I'm after for Z is (+) 0.7037
All my tools are always measured off the Z touch off gage on the right. The aluminum block equals the value of 4.0" above my Kurt Vises. I dont actually use a vise to do this because I dont always have a vise mounted to the table but want to maintain a value that always works.

I do however think it's silly that Haas does not have a feature that would allow me into input my (constant) off set value into the machine then simply measure the top of my part. It's seems like a no brainer but what do I know, I'm not a programmer.

For your current set up, all you need to do is put the difference in height between your tool touch off and the top of work into your work Z offset. It doesn't matter how long your indicator is; just the difference between the two touch off points.

But I think what you are getting at might be to turn on setting 64. Then you touch off your work, and the control uses that for the tool touch offs.

[QUOTE=Fletch_CNC;1837054]For your current set up, all you need to do is put the difference in height between your tool touch off and the top of work into your work Z offset. It doesn't matter how long your indicator is; just the difference between the two touch off points.

I looked that up, I don't think it's what I want to do.

Ah, I think I get it (it's early yet, and I haven't had any coffee) -- you want to be able to put your 3D indicator in, touch it off on the part, and input the value including the indicator length all at once. The effective result should be the difference between your tool touch off and the part top, one way or another. Ok, I understand the problem, but I can't think how to solve it with a constant input. I mean, you could put the constant into the Operator position screen when you start jogging, and then you'd get the difference when you touched off. But that requires entering the value every time. Barring using a macro program or something like that, I can't think of a quick way to do exactly what you want. You could make yourself a quick program to store on the control to use G10 to input your constant, maybe? Instead of doing the math and entering the value.

1 When you adjust the 3D tester on the base surface in the offset table, add the distance to the base surface on which you are setting up the rest of the cutting tools.
Let us assume that the tester is set to position number 1.

2 Write the following program
o1000
G49
# 5223 = # 5023- # 2001
M30

3 Touch the tester and workpiece surface.
4 Run the program.
If I am not mistaken in the G54 Z needed you will value.
Tomorrow I will try to work, if you have time.

Here's a good tip for using operator's coordinates on Haas to get results similar to G43:

To move the zero to tip of tool when using Operator's Coordinates:
Do a tool change to force the machine to its Z0.000 machine location
Use a calculator to find: - (Gz) - (Hz)
Enter this value as Z in operator's coordinate page & press Origin to set.

Example: G54z = -18.6245
H02 = 5.7300
-(-16.6245)-5.73 = 10.8945
Key in Z10.8945 as “origin” for operator's coordinate

The tip of the tool will now be zero in operator's coordinate page. I use this a lot when using the machine in manual mode. Also will work for you Haimer 3D taster.

Put a minus 4" in G52 Z Offset

Setting G54Z and Tool Offsets without a probing system.

Setting G54Z (Part in Vise for this example.)

Put Cursur to G54 Z offset Type in:

1) Distance from Table to vise bottom (where parallels sit)
2) Add Height Of Parallels
3) Part thickness minus amount you want to remove to clean up top of part.

Table to vise bottom = 2.875 (hit F1)
Height Of Parallels = 1.000 (hit enter to add)
Part Thickness = 2.000 (hit enter to add)
Amount to remove from top of part (establish z0) = (-) .025 (hit enter to add)
_________
G54 Offsett = 5.850
Set Tool Offsets

Set tools off machine table using a 1-2-3 block and the 2" side (hit tool offset measure)

Move cursor to G52 Z Offset. Type in (-) 2.00 (F1 to enter)

Note: The G52 command works differently depending on the value of Setting 33. This
setting selects the FANUC, HAAS, or YASNAC style of coordinates, which are listed below:

G52 SET LOCAL COORDINATE WORK OFFSET SHIFT VALUE FANUC
This code sets the origin of the local (child) coordinate system to the command location,
relative to the current work system origin. G52 is a non-modal, no motion code. The G52
coordinate system will stay in effect for all work systems until it is canceled. The G52 is
canceled when RESET is pressed and at the end of a program. It is also canceled during
a program by M30, G52, X0 Y0 Z0, or by a G92 command.


G52 SET LOCAL COORDINATE WORK OFFSET SHIFT VALUE HAAS
This code acts the same as in the Fanuc control except that G52 is not cleared at powerup,
RESET, or when an M30 is performed. It is canceled with a
G52, X0 and/or Y0 and/or Z0, or by a G92 command.

When you set up a new job just set the G54Z as above. The tool offsets will be good.

Setting G54Z and Tool Offsets without a probing system.

Setting G54Z (Part in Vise for this example.)

Put Cursur to G54 Z offset Type in:

1) Distance from Table to vise bottom (where parallels sit)
2) Add Height Of Parallels
3) Part thickness minus amount you want to remove to clean up top of part.

Table to vise bottom = 2.875 (hit F1)
Height Of Parallels = 1.000 (hit enter to add)
Part Thickness = 2.000 (hit enter to add)
Amount to remove from top of part (establish z0) = (-) .025 (hit enter to add)
_________
G54 Offsett = 5.850
Set Tool Offsets

Set tools off machine table using a 1-2-3 block and the 2" side (hit tool offset measure)

Move cursor to G52 Z Offset. Type in (-) 2.00 (F1 to enter)

Note: The G52 command works differently depending on the value of Setting 33. This
setting selects the FANUC, HAAS, or YASNAC style of coordinates, which are listed below:

G52 SET LOCAL COORDINATE WORK OFFSET SHIFT VALUE FANUC
This code sets the origin of the local (child) coordinate system to the command location,
relative to the current work system origin. G52 is a non-modal, no motion code. The G52
coordinate system will stay in effect for all work systems until it is canceled. The G52 is
canceled when RESET is pressed and at the end of a program. It is also canceled during
a program by M30, G52, X0 Y0 Z0, or by a G92 command.


G52 SET LOCAL COORDINATE WORK OFFSET SHIFT VALUE HAAS
This code acts the same as in the Fanuc control except that G52 is not cleared at powerup,
RESET, or when an M30 is performed. It is canceled with a
G52, X0 and/or Y0 and/or Z0, or by a G92 command.

When you set up a new job just set the G54Z as above. The tool offsets will be good.

New here and I don't know if this thread is still monitored but I have a question.

Firstly, I have many years setting up CNC mills, ALL of the mills I have run, Proto-Trak, Milltronics, Servo, Okuma. they are all simple like this:
All tools are set 4" off the table, using an EDGE tool setter set to match 2 123 blocks at 4"
All tools are set in a Coordinate System I never use to program (IE G111) (WCS#20 on Okuma)
I use a Haimer as T20 set to the 4" 123 blocks.

Then I to set the work coordinate, (G54) I use T20 to probe Z. TADA all is perfect, no math, no typing, no changes to any datum.

BUT, on this older HAAS Control from 2000, I read above, several varying methods with no solid results.
You should not have to use the 4" blocks, then Z then add/subtract.

I do not know what this mil is doing, since I have in the G Code T2 ramping from .100" to Z0", however the WORK G54 is going -2" or more below.
It's like the control can't even read G Code