[kentdesautel13]

I recently purchased a Haas Super Mini Mill, and I'm having problems trying to figure out how to get my G54 Tool offsets to work.

I am measuring my tools off of the top of the mill table, and then measuring my G54 Z-axis offset off of the top of the piece I want to mill.

So here are the steps I'm taking:

Measured Tools 1 & 2 off of the table.
Tool 1 ended up at –9.802
Tool 2 ended up at –9.306

Next using tool #1 I measured off of the top of the piece I want to mill.
That measured –5.8416 ( so I entered that into the G54 Z AXIS )

Next I keyed in my X & Y values into the G54

Next I ran the following code to see if the machine would bring me down near the X0,Y0,Z.25 position on the work piece.

I receive a Zero over travel range Error Message.

T1 M06
G0 G90 G54 X0 Y0
G43 H01 Z0.25
G28 G91 Z0

I have attached some screen shots.

On a side note, when I manually move the spindle down with tool #1 active It does show zero on all 3 axis when I get down to the zero position on the part, however when I load up tool #2 the z axis doesn't show zero when I get to the same place on the part... ( it appears it's still using the offsets from tool #1 )

Thanks,

Kent

Attachment 405968

Attachment 405970

Attachment 405972

[Machineit]

Your measurement off of the work piece should be a positive number to bring it up not more down. +5.8416.

I would suggest that for learning purposes, just touch your tools off the top or Z0 of the part and leave the "Z" G54 value at zero. Makes using just two tools so much easier and convenient.

[BlueChip]

One way to accomplish this :
(1) Measure your tools to the top of the table ... which in effect becomes Z0
(2) The distance in G54 Z is the difference between the top of the table and the Z zero surface of your part.

So in effect all the tools want to cut at the top of the table when G54 Z is zero ... but by adding a "work shift" in Z ... the distance from the top of the table to part zero ... you are shifting the Z0 by that amount.

Using this method you would always touch your tools to the top of the table no matter what ... and G54 would shift that Z0 a different amount for every job.
You can use your G43 H offset to make minor adjustments for each tool as necessary.

Hope this helps ....
Please check out our Real World machine shop software at Kipware® Software - Real World Machine Shop and CNC Software

[precisionmetal]

Kent,

Your G54 Z value will be POSITIVE, and it needs to be the DIFFERENCE between the value you see touching the table, and the value you see touching the top of your part.

In other words, if your tool #1 touches the table at an absolute value of -9.802, and that SAME tool touches the top of your part at an *absolute* value of -5.8416, then the DIFFERENCE between those two numbers needs to go in as a POSITIVE value in your G54 Z work offset.

9.802 - 5.8416 = 3.9604". Your G54 Z work offset should be +3.9604 . You can verify this by holding up your 6" scale and do a quick measurement from the table to the top of your part.


I assume you do not have a probe?

Please note: if you set the Z offset for tool #1 FIRST, and then use that same tool and touch the top of your part -- then... without moving that tool (it's in position touching the top of your part), you should be able to highlight the Z column in G54 on your work offset page, and push the "Part Zero Set" key (under the F4 key on your control), and that POSITIVE distance from table to top of your part should be entered into that Z offset value. That value should be the same as the difference calculation above.

PM

[kentdesautel13]

Thanks for all the help from all of you..... all of your suggestions fixed the problem....

Chips are flying once again...!