NOTE: If the fixture or workpiece requires you to adjust the C Axis to achieve the proper alignment for machining, use the following procedure to adjust and record the C-Axis work offset.

Setting the C-Axis Workpiece Orientation

Place the workpiece on the platter (workholding not shown). Adjust the C Axis until the workpiece is positioned to the same orientation established in the program. Typically, a reference feature on the fixture or workpiece is parallel to the X or Y Axis.

Navigate to [OFFSET] >Work. Scroll to the work offset value used in the program (G54 in this example).

Highlight the value in the C Axis column. Press [PART ZERO SET] to record the offset.

NOTE: Use this procedure if the WIPS probe is disabled.

 NOTE: Refer to the Haas Mill Operator’s Manual for basic offset and toolsetting methods.

X- and Y-Axis Zero Position

Jog the X and Y Axes to the zero position established in the program.

Navigate to [OFFSET] >Work. Scroll to the work offset value used in the program (G54 in this example).

Select the X Axis column of your work coordinate offset and press [PART ZERO SET] to set the X-Axis zero position.

Press [PART ZERO SET] again to set the Y-Axis zero position.

Determine a tool set plane to be used for setting all tool length offsets; for example, use the top surface of the workpiece.

See Example Tool Set Plane (Top of the Part).

Load the master gage tool included with WIPS into the spindle.

Make sure that the B and C Axes are at the same work zero point set earlier. (G00 G90 G54 B0 C0).

Select the Z AXIS column of your work coordinate offset.

Jog the Z Axis to the tool set plane. Make sure that the end of the gage tool you are using just touches the tool set plane. You will touch-off all of your tools on this surface.

Load the work probe into the spindle.

Make sure that the B and C Axes are at the same work zero point set earlier. (G00 G90 G54 B0 C0). Refer to the Set the B-Axis Work Offset and Set the C-Axis Work Offset sections if these values are not correct.

Set the X- and Y-Axis offsets using the standard WIPS templates as appropriate. Refer to the WIPS manual for more information.

Position the work probe tip approximately 0.25" (6 mm) above the Z-Axis zero surface.

Navigate to OFFSET Work. Scroll to the work offset value used in the program (G54 in this example).

Press the right cursor arrow until you reach the Probe Action sub-menu.

Type 11, and then press ENTER to assign the Single Surface Probe Action to the offset.

Press PART ZERO SET to move to VPS.

Select the Z Variable.

Type -.5 (or -12 if the control is set to metric measurements), and then press ENTER.

Press CYCLE START. The probe measures the distance to the top of the part and records the value in the Z Axis column work offset for G54.

Use the tool setting probe to set each of your tool length offsets.

When safe zones are active there are limitations to certain axis movements to prevent crashes from occuring. The message box "RESTRICTED ZONE REACHED" will appear any time a user reaches these limits when hand jogging. When the machine is commanded a movement by program and the machine reaches a Safe Zone the machine will alarm out with a Alarm 9108 – Potential Collision Detected  and the "RESTRICTED ZONE REACHED" message box will also appear. 

If this message box appears in an area it should not, please re-calibrate Safe Zones.

If this issue persists please contact the Haas Service department. 

Safe Zone parameter 2159 MACHINE GEOMETRY FILE TYPE [3] will enable and disable safe zone parameters. Machines built after 1/1/2022 and software version 100.20.000.1200 or higher will receive the machine with the function enabled.

NOTE: This parameter can be found by pressing [DIAGNOSTIC] and navigating to parameters [1] and to the factory parameter tab [2] using a service key. 

Machines that update to the latest configurations after 1/1/2022 and upgrade to software version 100.20.000.1200 or higher will have the feature but it will not be enabled. 

After running the safe zone calibration program settings 378-380 will be populated. Below is a brief description of what each of the settings are

378 Safe Zone Calibrated Geometry Reference Point X - Defines the X reference point for all safe zone geometry (For UMCs it is the center of the C Axis Platter.)

379 Safe Zone Calibrated Geometry Reference Point Y - Defines the Y reference point for all safe zone geometry (For UMCs it is the center of the C Axis Platter.)

380 Safe Zone Calibrated Geometry Reference Point Z - Defines the Z reference point for all safe zone geometry (For UMCs it is the top of Platter or PP table.)

By default Setting 408 Exclude Tool From Safe Zone will be turned OFF.  This setting, if left OFF, will allow the machine to account for the tool in the Safe Zone function. This will require that all tool offsets to be set correctly for this function to work properly. 

If the user needs to drill or tap a fixture hole in the platter then the safe zone must be disabled by changing Setting 408 Exclude Tool From Safe Zone to a value of ON. 

NOTE: A watermark will appear in the program box when the Setting 408 is set to ON.

A collision between elements in group 1 and group 2 can occur at non-B=0 angles when moving in B or the Z-Axis.

Another collision between elements in group 1 and group 2 can occur at non-B=0 angles when moving in B or the X axis.