[l u k e]

Another newbie question, the Haas manual is no help so here I am (again). I'm a little confused on setting the “work piece” z height (Not the tooling).

I purchase the Pro Touch Off Gage>



I touched off all my tools with the Pro Touch off Gage sitting on top of my vice which will place the tools 4" above that point. My work piece will be below that, which seems to be the general consensus on how to do it.

What I'm unsure of is inputting the Z height of the work piece. I have two guesses on how to do it, but it's only a guess.

Guess #1
Would I just measure the difference in height between the “Z setter zero” and the top of the part, and then input that difference in the Z height for the work offset?
In other words if my part was going to be G54 and it happens to be exactly 2.2000" lower than the zero height on the z setter, would I would type in -2.2000 for Z in G54?

OR

Guess #2
The manual only has one suggestion on this and it is to touch off the tools to the top of the part, this leads me to my second guess.

Using the same scenario with my work piece being 2.2000 below my Z setter zero, would I simply edit the tools by adding 2.2000 to the measured height? (This doesn’t seem to be much of a shortcut using a z setter)

I just can’t figure out how else the control would know the relationship between the tool Z height and the part Z height.

[MSFAB]

I do the same thing all day long but use a 1 inch tool setter.
1st measure the distance from the top of the vice to the top of the part using the machine and a dial indicator. Insert that into the z value for g54 then minus the hieght of your tool setter.

Example
Difference between vice and part
+2.5
Tool setter 4.0
Enter 2.5 f1 Into g54 z value
Then -4.0 write enter button
You will get -1.5 for z offset
Then always check the first tool with a 123 block

Hope this helps
Then

Sent from my SAMSUNG-SGH-I897 using Tapatalk

[MSFAB]

Assuming your setting the tool setter on top of the vice if not measure from where ever the tool setter is sitting. I use a mitutoyo setter
Cheers
Marcus

Sent from my SAMSUNG-SGH-I897 using Tapatalk

[l u k e]

I do the same thing all day long but use a 1 inch tool setter.
1st measure the distance from the top of the vice to the top of the part using the machine and a dial indicator. Insert that into the z value for g54 then minus the hieght of your tool setter.

Example
Difference between vice and part
+2.5
Tool setter 4.0
Enter 2.5 f1 Into g54 z value
Then -4.0 write enter button
You will get -1.5 for z offset
Then always check the first tool with a 123 block

Hope this helps
Then

Sent from my SAMSUNG-SGH-I897 using Tapatalk

So you're saying that guess #1 is correct, I just input the difference and don’t reset all the tools z height like guess #2 ??

[MSFAB]

Yes guess 1 is correct. The leave tools set where there at. What size Haas are you running?

Sent from my SAMSUNG-SGH-I897 using Tapatalk

[l u k e]

VF2

[MSFAB]

Hey Luke I took a short video on my phone so i apologize for the crappy resolution. I took it at work to show the process. The tool setter is to the left. I set the tools to that which is 1 inch.
I press the Mdi button then the hand jog button to zero the dro for measurement

[nomedia="http://www.youtube.com/watch?v=HWEb2LsAAOs"]YouTube - Haas mini z fixture set[/nomedia]
Cheers Marcus

[l u k e]

I believe I understand the basics of the actual measuring; I was more inquiring about the “value” that was put into ‘G54- Z’ for the part height.

I have a Haimer 3D sensor that will remain in the tool changer on my machine.



I have set a tool height for the Haimer off the same block that I calibrated the Edge Z Setter with.



From the help I’ve received I’m under the impression that all I have to do is load the Haimer in the spindle touch off the Z height of my part; subtract the calibrated Haimer Z height from the part Z height put the difference in the Z setting for G54 (G54-G59 whichever I use).

The math:
'Haimer Z' -7.9404
'Part Z' -9.9549
'G54 Z control entry' -2.0145

Is that correct?

[MSFAB]

Yes that is correct. You got it.

Sent from my SAMSUNG-SGH-I897 using Tapatalk

[l u k e]

Sweet!

:cheers:

[Pondo]

Make sure setting 64 is "OFF" if you are touching off tools anywhere except the part Z0 surface.
If it is on, it will apply the G54 Z offset to the touchoff.
You have it figured out correctly. You can touch off tools on any surface, then put the G54 Z offset as the distance from that surface to the Z0 surface of the part. + or - does not matter. The controller adds that # to the tool offset position to figure out where the tool tip is when running a program.

[Pondo]

Another way to set the G54 Z0 is to use the Haimer to measure it. Just like you would with a regular indicator in the spindle.
Set the Haimer to 0 on the top of the 1-2-3 block where you have the red arrow and set the user Z display to 0.
Move the Haimer to set 0 on the part's Z0
The display Z0 is the G54 offset (the distance from the tool touchoff to the part Z).
You can use the Haimer (or an indicator) to measure very exact sizes in X and Y this way too, using the machine like a budget CMM.

[l u k e]

Another way to set the G54 Z0 is to use the Haimer to measure it. Just like you would with a regular indicator in the spindle.
Set the Haimer to 0 on the top of the 1-2-3 block where you have the red arrow and set the user Z display to 0.
Move the Haimer to set 0 on the part's Z0
The display Z0 is the G54 offset (the distance from the tool touchoff to the part Z).
You can use the Haimer (or an indicator) to measure very exact sizes in X and Y this way too, using the machine like a budget CMM.

Not sure if I completly understand.

Let me use my original explanation to see if i get it.

Are you saying I can also do this:
(Let me use my original explanation to see if i get it.)

The math:
'Haimer Z' -7.9404 (When I touch this off I can change the setting input to 0.0000)
'Part Z' -9.9549 (Using my original math this move would be -2.0145)
'G54 Z control entry' -2.0145 (Just hit the write/enter button for Z, entering -2.0145)

[l u k e]

Ok I'm stumped!
I know how to measure the part/tools and do understand the G54 work offset.
My problem is my control will not let me "type in" any values.
The only way it is letting me put a measurement into Z is by using the "Tool Offset Measure" or "Part Zero Set" buttons.

I know that my part is 2.4425 below the Z height of my tooling.

My problem is I can not "type in" -2.4425 into G54 Z.

I wonder if there is a setting that is locking me out???????

[Geof]

Setting 119 is offset lock in my manual.

[l u k e]

I did check 119 and it was off. With the on setting it will lock out any input, no question about that, I checked it.

But, I just figured it out 60 seconds ago.
If the value in G54 Z is anything other than 0. a value can not be typed in.
Zero it out and it works fine.

[l u k e]

OK here is another inquiry.
I want to set my Haimer 3D edge finder "tool height to Z zero" in the control which is the Z location for my end mills. (Using the top of the block I use to zero out my z guage to do so)





I have the same problem as above; the control will not take any data input except from the tool and work measure buttons on the control. (Even if I start from 0. like is necessary in G54 Z inputs)

The idea of setting it to zero at the end mill height is I wouldn't have to do any math to find the setting for G54 Z for work coordinates.
I believe that Pondo suggested this is possible.
???????

[Machineit]

If you want to change the tool or part offsets you can do it three ways that I know of.

1. Set them by touching of tools or part edges and hit tool or part off set measure.

2. To add or subtract to a number that is already entered, such as adding (1.0) or subtracting (-1.0) write it then hit the write key. (The same key you enter code into MDI with)

3. To enter your own specific number, enter the number such as 10.9765 and then hit the F1 key. This will change whatever is entered to what you enter.

So, with the write key you can add or subtract and with F1 you can enter your own number.

Just as an example, if you need tool one to go .001 deeper, you can add .001 to the tool offset with the write key, or you can add it to the wear adjustment for that tool.

Mike

P.S.: I would recommend being careful with adding your own numbers and make sure you single block your first programs and have the rapid set to 5%. It is very easy to enter the numbers wrong!

[l u k e]

Thank You!

I will give it a try! (F1)

I'm currently only interested in setting up my Haimer at Z0 which will be the same Z offset my tooling. The idea being than when I touch off the top of my part for G54 Z I can hit the work measure without doing any math... (At least in theory, I'll have to play around with it)

[stan_rg41]

I still can't get my head around this, must be my age.

What I want to do, is set up all my tools with the tool setter and enter the values in their appropriate tool offset boxes, then put the tool setter to one side and forget about it.

My preferred set up for setting the billet Z0 is to clock the top of the parallels then the top of the vice back jaw and calculate the slips required to give me my equivalent billet Z0.

I then want to bring one of the tools down to touch the slips, preferably one that's unlikely to break or get damaged eg. a deburring tool, we'll call it T8.

My question now is, from here, how do I arrive at my G54 Z offset?

What numbers and displays do I need to be looking at, what calculations do I need to do and what buttons do I need to press?