Height Offset Problem

[dpascucci_support]

To explain what Uwe was saying, if you look back at your videos, the first time you probed, you can see the tool loaded in the top-right reads T4 H100, so it's using height offset 100 which is your probe. But the second probing cycle, the tool loaded reads T4 H4, using height offset 4. So the machine thinks the tool is about 3 inches higher than it actually is because it thinks T4 is there.

[RJS100]

Thanks... that helps. But why is this happening. Why would this change after I ran simple gcode?

[cnckeith]

you may find swissi's probe app useful as it hold's your hand through the various methods and setups when it comes to all things probes.
https://centroidcncforum.com/viewtopic.php?f=60&t=6149

[swissi]

Thanks... that helps. But why is this happening. Why would this change after I ran simple gcode?

Look at the code you posted:

Code: Select all

N30 T4 M6
N35 S3000 M3
N40 G54
N50 G0 X2.19 Y-0.6574
N55 G43 Z0.4 H4

On line N30 Tool T4 is loaded and on line N55 the Tool Height Offset H4 that is associated with T4 is activated with G43 H4.

When your job ends CNC12 is most likely still set at T4 H4 when you look in the top center of the CNC12 screen. Now when you load your Touch Probe with the command T100 M6, CNC12 will show T100 H4 because CNC12 does not automatically switch the Tool Height Offset to H100, you must command that with a G43 H100 and then CNC12 will show T100 H100 and your height probing with the TP will show the correct coordinates.

Not to complicate things even more, but you need to be aware that any of the 200 Height Offset values (H1 - H200) can be assigned to any of the 200 Tool numbers (T1 - T200). So in theory, you could assign H10 to T20 as an example iand n in this case you would need to issue the command T20 G43 H10.

The command G49 will turn of Tool Height Offsets and CNC12 will show T4 H-- as an example.

As Keith mentioned, the ProbeApp does a lot of guidance to setup tool height offsets correctly. The ProbeApp does have a Setup Questionnaire that will ask you questions about your machine and will setup everything based on your answers.

Hope this helps.

-swissi

[CNCMaryland]

I have my Parameter #3 set to 0.

[RJS100]

Swissi,

Thanks for the great explanation. I am ordering your probe app NOW!

[suntravel]

Thanks... that helps. But why is this happening. Why would this change after I ran simple gcode?

This is because there is no G49 at the end of the g-code
G49 unloads the current tool offset height, so T4 H4 stays active.

Pls, work through the manual, helping you to understand what the UI tells you and how g-code works.

Only using CAM like fusion will left you several times with some ??? over your head

Uwe

[RJS100]

Thank you. I started this 2 years ago, never had touched a machine before, converted a machine, learned lots of Fusion 360. Machined some nice stuff... Next stop... gcode.

[suntravel]

Starting with fusion is like learning to run before learning to walk

Uwe