What's new
What's new

Haas VF4D Pre-NGC Setting Z Work Offset

Diemetinc

Plastic
Joined
Mar 30, 2024
Location
Florida
Good Evening Everyone , hopefully someone on here can help me out .
I Know setting Z Offset has been discussed to death and everyone has different methods and i know this but i need help with how i normally do this
I Have inherited a 2001 Pre-NGC Haas VF4 with a workshop i have purchased. the previous owner always set Z by touching off each tool on the work piece, which is fine if doing a few jobs with limited tools. We are now doing lots of one offs with multiple tools so do not want to spend all day touching off tools.

Method i always used , (No Haas experience BTW) here is an example of what happens
Make Sure G54 Z offset is Zero
Touch off T1 -T3 on table and set with tool offset measure button (T1= -17.3660", T2 = -18.3260", T3 = -16.6647)
use hammier in T4 using operator Posit page measure from table to top of work (5.535")
set G54 Z offset to +5.535"
Now go back to Posit Page and touch the tools on the top of the workpiece and it gives G54 Z values as the original Tool Length Settings ?? where as it should give G54 Z0 ??

I have followed numerous tutorials and cannot work out what I'm doing wrong or what setting/Parameter is not enabled ???

If I set G54 Z Offset to 5.535" before i set tool lengths on the table it just adds this value to the measured tool length , with the same outcome

TIA
Sean
 
I believe you're looking for setting 64 in the manual:

64 - T. OFS Meas Uses Work
This setting changes the way the Tool Ofset Mesur (Tool Offset Measure) button works. When this is On, the
entered tool offset will be the measured tool offset plus the work coordinate offset (Z-axis). When it is Off, the
tool offset equals the Z machine position.
 
You would have to MDI the tool offset to be active in order for the G54 position display to read Z0 when touching the part.
 
What Donkey said...
I use this
And this
And a 2-3-4 block
I do touchoffs on the back of my vise but the location is up to you
4" off the top of the vise with the items above is Z0.
 
Last edited:
Thank you all for your helpful replies here is what i have done this morning
Made sure Setting 64 is on ( it is by Default )

g54 Work Offset set to Z = 0 before i set tool lengths
set T2, T3 and T4 to Table with tool offset measure button ( T2 = -18.3260, T3 = -17.3660, T4 = -19.1400)
Set G54 Z offset to 3.000
Run MDI G54 , G43 Z0 with each tool
From the Position Screen measure distance to table
T2 @ G54 Z0 =3.0010" from Table
T3 @ G54 Z0 =(3.000" - 0.9660") = 2.034" from Table
T4 @ G54 Z0 =(3.000" + 0.805") = 3.805" from Table

the differences in distance to table at G54 Z0 for any tool but T2 is the difference in tool length from T2 it seems ??

TIA
 
If I do not have WIPS I use a standard to set my tools to as well as a specific work offset. Example:

Last shop I worked where I done this I made a 2" x 4" round standard to touch off to.
Use edge finder as touch off tool for work offset and tool touch off and leave in the machine as T1
first I touch off the edge finder in z on my standard and set my z to an off set that I don't normally use. Here it was G59.
Then i touch off all my tools to the same standard in Z
Now all your tools are touched off to the same standard.
Now all you got to do is use the same edgefinder to touch off your workoffsets for your job in xyz.
If you break a tool just put the standard back in and touch of the new tool the same way using G59.
 
Thank you all for your helpful replies here is what i have done this morning
Made sure Setting 64 is on ( it is by Default )

g54 Work Offset set to Z = 0 before i set tool lengths
set T2, T3 and T4 to Table with tool offset measure button ( T2 = -18.3260, T3 = -17.3660, T4 = -19.1400)
Set G54 Z offset to 3.000
Run MDI G54 , G43 Z0 with each tool
From the Position Screen measure distance to table
T2 @ G54 Z0 =3.0010" from Table
T3 @ G54 Z0 =(3.000" - 0.9660") = 2.034" from Table
T4 @ G54 Z0 =(3.000" + 0.805") = 3.805" from Table

the differences in distance to table at G54 Z0 for any tool but T2 is the difference in tool length from T2 it seems ??

TIA
G43 Hhh Z0
 
Thank you all for your helpful replies here is what i have done this morning
Made sure Setting 64 is on ( it is by Default )
I believe you want 64 to be off. If you're using a presetter or the table or whatever as your master zero, all tool lengths should be from that datum. Work coordinate should not factor in. Work coordinate Z should be the difference between whatever that datum is and the desired work zero.

Example: you touch all the tools off the table. All tool lengths represent that distance. Now you have work sitting on parallels in a Kurt vise. The G54 distance will be the positive distance from the table to the top of the parallels (+3.217 or whatever).

When 64 is turned on it changes it so you're supposed to touch the tool off of the parallels instead of the table. The problem is: how did you determine the distance from the table to the top of the parallels. If you were sloppy and/or didn't us an indicator to move and record that distance, you've added error to your offset.
 
If you need to replace a tool during a run refer to Mr Hotey’s post #9

Also , to OP
If you’re doing a lot of one offs that need different tools the reality is you will always be touching off tools. You need to standardize the way you feel it should be done.
 
I believe you want 64 to be off. If you're using a presetter or the table or whatever as your master zero, all tool lengths should be from that datum. Work coordinate should not factor in. Work coordinate Z should be the difference between whatever that datum is and the desired work zero.

Example: you touch all the tools off the table. All tool lengths represent that distance. Now you have work sitting on parallels in a Kurt vise. The G54 distance will be the positive distance from the table to the top of the parallels (+3.217 or whatever).

When 64 is turned on it changes it so you're supposed to touch the tool off of the parallels instead of the table. The problem is: how did you determine the distance from the table to the top of the parallels. If you were sloppy and/or didn't us an indicator to move and record that distance, you've added error to your offset.
Thank You DH , yes i worked this out earlier so have turned S64 off now.
I have an SPI Tool setter on the table and use Haimer 3d to set the XYZ offsets .
 
If you need to replace a tool during a run refer to Mr Hotey’s post #9

Also , to OP
If you’re doing a lot of one offs that need different tools the reality is you will always be touching off tools. You need to standardize the way you feel it should be done.
Thank you again for your help post #9 Noted.
We are trying to bring in a standard method of work regarding tool length and offsets as you suggest. we are printing tool tags for all our holders as we speak so that we can fill in tool data and the measured offset for each tool and also know what tools are in the ATC .
I think we have enough Cat 40 tool holders to cover 90% of the jobs we are currently doing , with only Taps and Drills needing to be changed out regularly , so rather than touching off 7 or 8 tools on the job surface we will only have to touch a few off the tool setter.
 








 
Back
Top