Haas ST30Y Y Axis issue in code ouput

[dtoniob]

Very simple. Code generated with the latest Haas ST30Y post throws an error for unknown m code M154 which the manual says is for C axis. Correct M codes for live tools according to the manual are M133/134/135 for foward reverse and stop on the Y axis controls. Im try to do a simple bore function for a hole. every other part of the turning cycles works. i wrote basic warmup program for the live tools and the same issue happened i had to edit all the M154 to M133 to get them to work. Ive selected tool orientation when generating the bore function and that didnt help as someone told me I had to select orientation when using live tools as well.

[seth.madore]

M154 is the C axis control. I'm assuming your machine has a C? 

The current ST30Y post is setup to also use M133/4/5 for live tools:

 case "STOP_SPINDLE":
    if (machineState.liveToolIsActive) {
      machineState.liveToolIsActive = false;
      return mFormat.format(135);
    } else if (machineState.mainSpindleIsActive) {
      machineState.mainSpindleIsActive = false;
      return mFormat.format(5);
    } else if (machineState.subSpindleIsActive) {
      machineState.subSpindleIsActive = false;
      return mFormat.format(g14IsActive ? 5 : 145);
    } else {
      return undefined;
    }
  case "START_LIVE_TOOL_CW":
    machineState.liveToolIsActive = true;
    return mFormat.format(133);
  case "START_LIVE_TOOL_CCW":
    machineState.liveToolIsActive = true;
    return mFormat.format(134);

Tool Orientation is only required if you are working on an axis that is not the Z; so if you had to drill a cross hole or mill a pocket along the XY axis, you would use orientation.

Do you have any code that you HAVE run with live tools?

[dtoniob]

The tools i created in the tool library for milling i check the selection box for live tooling but the gcode is still created with M154 instead of M133 like it supposed. I created a basic warmup program for the live tools to break them in originally and that works. Here is the current posted code from fusion as soon as it reaches line 13 on the control i get an error for Unknown M Code for M154

%
O01001 (1001)
G98 G18
G20
G50 S4500
G53 G0 Y0.
G53 X0.
G53 Z0.

(Bore4)
T707
(Axial Milling 3/8")
M154
G98

[seth.madore]

What year is your ST30Y, brand new? This is taken right from the NGC Lathe manual for Haas:

Are you in single block when it alarms out, or executing from the start and waiting for the alarm? The reason I ask is this: If single block is on, it will (should) execute one line at a time and not load any future lines into it's buffer. If you've executed the program with Single Block off, there's a high possibility that it's actually alarming out on a line further down. Can you share the actual program you are alarming out on?

 

[dtoniob]

The lathe is brand new built about a month ago with the NGC controller. I tried single block and it does alarm out exactly at the line with M154.  Sample program attached below along with pics from my manual.

[seth.madore]

The sample program you shared is the same one as you shared initially. Can you share the program that's actually alarming out?

[seth.madore]

In your second picture, it's listed as "optional". I'm assuming that if you have a Y axis, you must also have a C axis, no? Otherwise, you have no ability to do Y axis work? So is it optional still on a Y axis machine from Haas?

[dtoniob]

My Lathe has a BMT style turret maybe that has something to do with it but NONE of the C axis M codes work on my controller because both my radial and axial milling heads only operate using the Y axis codes. I verified this when i had to run a break in program for all 6 of my milling heads and in the code i created M154 was no-go but M133/134/135 all worked fine on both radial and axial tools. 

[seth.madore]

M154 controls the C axis, which is your chuck/main spindle. This has nothing to do with your live tooling, just the chuck.

Apples and oranges

What controls the clamping/unclamping and indexing of your workpiece?

[Anonymous]

M154 is c axis engaging lock. 

[rhedges]

maybe on the features tab on the diagnostics page the c axis may not be selected ive seen that before M154 is c axis engage and has been on all haas controls there is nothing wrong with the fusion post

[dtoniob]

the C axis was disable in the software on the control. got it updated and everything works fine