[rdykstra8]

I am having trouble with the H and T not matching in the code.

I know what tool number I want to use and I use G54 for the offset, but I do not know what to put for the H number. Tried putting the H number the same as the tool number (T) but that was not working.

I am used to having different G54 G55 etc... for the tool length compensation on the Haas Lathe we have, but never had to use H to define the tool length compensation.

This is the first Haas Mill that we have purchased and I appreciate any help with this problem.

[Superman]

The tool length call-up is activated with G43 Hxx Zzz where xx is the address of the register that holds the length value, & zz is the plane that you want the tool tip to stop at.

ie

T1 M6
G54 G0 X0. Y0.
S1000 M3
G43 H1 Z1.
G1 Z-zz Fff
G1 G41 D1 X1. Y1. 
....
G1 G40 X0. Y0.
G0 Z1.

Diameter offset is called using a Ddd & is activated with a G41 or G40, & de-activated with a G40....these can only be used on a linear move, never on an arc

[obiwon]

You do need to callout G43 H & D tool# to activate the tool offsets. In the case of using G12 and G13 , G41 G42 cutter comp is not required. But you do need to have the D tool # called out and the corrisponding diameter/radius in your tool offsets.. When you do arc moves using G41 G42 cutter comp , though not needed, it sure makes things easier.
So You touch EACH tool off on your part as apposed to just tool#1 on the lathe. In your tool offsets page each tool height is recorded using the tool offset measure button.
While on your tool offsets page, curser too the proper tool#... JOG that tool to touch the part....Press "tool offset measure" to record the tool height...press "next tool".... then jog that tool to the top of your part..etc
After doing that your program will look something like this;


T1 M06 (CD)
G00 G54 G90 G43 H1 D1 X0 Y0
S2000 F25.
G00Z .100 ( TOOL#1 IS NOW .100 FROM THE TOP OF PART)
M03
MO8
(REST OF PROGRAM FOR TOOL #1)

T2 M06 (DRILL)
G00 G54 G90 G43 H2 D2 X0 Y0
S2000 F25.
G00Z .100 ( TOOL#2 IS NOW .100 FROM THE TOP OF PART)
M03
MO8
(REST OF PROGRAM FOR TOOL #2)

Hope that helps answer you question

[miljnor]

you can also turn that agreement off in the settings. incase you have multiple offsets to 1 tool...which I have done in the past.

[Machineit]

you can also turn that agreement off in the settings. incase you have multiple offsets to 1 tool...which I have done in the past.

I would definitely not do this with a person who does not understand the system in the first place. Many bad crashes will happen.

Mike

[haastec]

I would definitely not do this with a person who does not understand the system in the first place. Many bad crashes will happen.

Mike

Yes! Yes! Yes!
Understand how the machine works and EXACTLY what you are telling the machine to do before disableing any safety type features.