8.1 Overview

Part Setup

Correct workholding is very important for safety, and to get the machining results that you want. There are many workholding options for different applications. Contact your HFO or workholding dealer for guidance.

8.2 Jog Mode

Jog Mode

Jog Mode allows you to jog each of the axes to a desired location. Before jogging the axes it is necessary to home (beginning axes reference point) the axes.

To enter jog mode:1. Press [HANDLE JOG]. 2. Pick an increment speed to be used while in jog mode ([.0001], [.001], [.01] or [.1]). 3. Press the desired axis ([+X], [-X], [+Z], or [-Z]) and either press and hold these axis jog keys or use the [HANDLE JOG] control to move the selected axis.

8.3 Tool Offsets

Tool Offsets

The tool offset behavior has been modified on Haas machines in the following ways:

  • By default tool offsets will now always be applied, unless a G49/H00 (Mill) or Txx00 offset (Lathe) is explicitly specified.

Press the [OFFSET] button to view the tool offset values. The tool offsets can be entered manually or automatically with a probe. The list below will shows how each offset setting works.

1. Active Tool: - This tells you which position is active turret.

2. Tool Offset (T) - This is the list of available tool offsets. There is a maximum of 99 tool offsets available.

3. Turret Location- This column is used to help the operator remember which tool is on the turret station. This is useful when you have a tool holder that has tools mounted on the front and on the back. You want to remember what offset each of the tools is using and where it is located.

4. X and Z Geometry - Each offset contains values for the distance from machine zero to the tip.

5. Radius Geometry - This offset is used to compensate for the radius on the tool tip when cutter compensation is used. Check the radius specification on the tool inserts and enter the value on this offset.

6. Tip Direction - Use this to set the direction of the tool tip when cutter compensation is used. Press [F1] to view the options.

7. These functions buttons allow you to set the offset values. Pressing [F1] enters the number in the selected column. Entering a value and pressing [ENTER] adds the amount entered to the number in the selected column. 

8. X and Z Wear Geometry - The values entered here are intended for minute adjustments to offset that are required to compensate for normal wear during the course of a job.

9. Radius Wear - The values entered here are intended for minute adjustments to offset that are required to compensate for normal wear during the course of a job.

10. Tool Type - This column is used by the control to decide which probe cycle to use to probe this tool. Press [F1] to view the options.

11. Tool Material - This column is used for calculations by the VPS feeds and speeds library. Press [F1] to view the options.

12. Live Tool Radius - This offset is used to compensate for the radius on the live tool tip. Check the radius specification on the tool inserts and enter the value on this offset.

13. Live Tool Wear - The values entered here are intended for minute adjustments to offset that are required to compensate for normal wear during the course of a job.

14. Flutes - When this column is set to the correct value, the control can calculate the correct Chip Load value displayed at the Main Spindle screen. The VPS feeds and speeds library will also use these values for calculations.

Note: The values set on the Flute column will not affect the operation of the probe.

15. Actual Diameter - This column is used by the control to calculate the correct Surface Speed value displayed at the Main Spindle screen.

16. Approximate X and Z - This column is used by the ATP or Tool Setting Probe. The value in this field tells the probe the approximate position of the tool being probed.

17. Approximate Radius - This column is used by the ATP probe. The value in the field tells the probe the approximate radius of the tool.

18. Edge Measure Height - This column is used by the ATP probe. The value in this field is the distance below the tip of the tool that the tool needs to move, when the edge is probed. Use this setting when you have a tool with a large radius or when you are probing a diameter on a chamfer tool.

19. Tool Tolerance - This column is used by the probe. The value in this field is used for checking tool breakage and wear detection. Leave this field blank if you are setting the length and diameter on the tool.

20. Probe Type - This column is used by the probe. You can select the probe routine you want to perform on this tool. Press [X DIAMETER MEASURE] to view the options.

8.4 Set A Tool Offset

Set a Tool Offset

The next step is to touch off the tools. Doing this defines the distance from the tip of the tool to the side of the part. This procedure requires the following:

  • An O.D. Turning Tool
  • A work piece that fits in the chuck jaws
  • A measuring tool to inspect the workpiece diameter

For information on setting up Live tools, refer to Programming Live Tooling section for more information.

1. Press [OFFSET]. Press [HANDLE JOG].

2. Load an O.D. turning tool into the tool turret. Press [NEXT TOOL] [F] until it is the current tool.

3. Clamp the workpiece in the spindle.

4. Press [.1/100] [B]. The axis selected moves at a fast rate when the handle is turned.

5. Close the lathe door. Type 50 and press [FWD] for the spindle to start.

6. Use the turning tool loaded in station 1 to make a small cut on the diameter of the material clamped in the spindle. Approach the part carefully and feed slowly during the cut.

7. After the small cut is done, jog away from the part using Z-Axis. Move far enough away from the part so that you can take a measurement with your measuring tool.

8. Press Spindle [STOP] and open the door.

9. Use the measuring tool to measure the cut made on the workpiece.

10. Press [X DIAMETER MEASURE] [D] to record the X-axis position in the offset table.

11. Type the workpiece diameter and press [ENTER] to add it to the X-axis offset. The offset that corresponds to the tool and turret station is recorded.

12. Close the lathe door. Type 50 and press [FWD] for the spindle to start.

13. Use the turning tool loaded in station 1 to make a small cut on the face of the material clamped in the spindle. Approach the part carefully and feed slowly during the cut.

14. After the small cut is done, jog away from the part using X-axis. Move far enough away from the part so that you can take a measurement with your measuring tool.

15. Press [Z FACE MEASURE] (E) to record the current Z position in the offset table.

16. The cursor moves to the Z-axis location for the tool.

17. Repeat all of the previous steps for each tool in the program. Do tool changes at a safe location with no obstructions.

8.5 Work Offsets

Work Offsets

Press the OFFSET, then the F4 to view the work offset values. The work offsets can be entered manually or automatically with a probe. The list below will shows how each work offset setting works.

1) G Code - This column displays all the available work offset G-codes. For more information on these work offsets, refer to the G52 Set Work Coordinate System (Group 00 or 12), G54 Work Offsets, G92 Set Work Coordinate Systems Shift Value (Group 00).

2) X, Y, Z, Axis - This column displays the work offset value for each axis. If rotary axis are enabled the offsets for these will be displayed on this page.

3) Work Material - This column is used by the VPS feeds and speeds library.

4) These functions buttons allow you to set the offset values. Type in the desired work offset value and press [F1] to set the value. Press [F3] to set a probing action. Press [F4] to toggle from work to tool offset tab. Type in a value and press Enter to add to the current value.

8.6 Set A Work Offset

Set a Work Offset

Your CNC control programs all move from Part Zero, a user-defined reference point. To set Part Zero:

  1. Press [MDI/DNC] to select Tool #1.
  2. Enter T1 and press [TURRET FWD].
  3. Jog X and Z until the tool just touches the face of the part.
  4. Press [OFFSET] until the Work Zero Offset display is active. Highlight the Z Axis column and G-code row that you want to use (G54 recommended).
  5. Press [Z FACE MEASURE] to set part zero. 
Feedback