Lathe Programming

Typical Lathe Program Process 

For a part with internal boring and external grooves and/or threading

1. Rough Facing/Rough Turn OD

2. Drilling for boring tool

3. Rough Bore

4. Finish Face/Finish Turn OD

5. OD Grooving

6. External Threading

7. Parting

Lathe Programming Workbook

Haas Lathe Programming Workbook

Startup

G28 U0. W0. (First line: Always go home in case last program stopped unexpectedly such as hitting e-stop, power failure, etc.)

G20 (Inches)

G18 (Sets X-Z plans for all G02/G03 moves)

G40 G54 G80 G99 (SAFETY BLOCK: CANCEL TNR, CANCEL CANNED CYCLE, FEED PER REV)

G50 S3500 (sets maximum rpm)

Tool Change

*see note above about G28 U0. W0.

T0101  (M06 NOT NEEDED, TOOL #1 CALLED WITH ITS OFFSET 01)

Spindle

G97 S500 M03 (Direct rpm input mode - sets spindle speed at 500 rpm and turns on spindle)

G96 S500 (uses constant surface speed)

G99 sets Feed per Rev mode

M03 spindle on forward (clockwise as viewed looking from the chuck towards the tailstock.  If you're standing at the operator panel position and looking at the spindle, it will appear counter-clockwise)

M05 Spindle Stop

Going Home

G28 U0. (Home along X-axis)

G28 W0. (Home along Z-Axis)

G02/G03 Circular Interpolation

On a slant-bed lathe G02/G03 may behave reversed from what you may expect.  If you notice that we are looking at the underside of the cutting tool what standing at the operator position.  You have to visualize the tool path from the back side on slant bed lathes with the chuck on the right not to the left.

G70 Finishing cycle

This command is used after the following command, G71, to finish the part.  It will make use of the same P & Q code blocks describing the part profile.

G70

P - Starting Block number of path to rough

Q - Ending Block number of path to rough

F - Feed rate

example: G70 P100 Q200 F0.004

G71 Roughing Stock Removal Cycle

Haas Service notes on G71

* D - Depth of cut for each pass of stock removal, positive radius (Only use when using one block G71 notation)

* F - Feedrate in inches (mm) per minute ( G98) or per revolution ( G99) to use throughout G71 PQ block

P - Starting Block number of path to rough

Q - Ending Block number of path to rough

* U - X-axis size and direction of G71 finish allowance, diameter

* W - Z-axis size and direction of G71 finish allowance

* indicates optional

Note: G18 Z-X plane must be active for using G02/G03

• • Haas Tip of the Day Mastering G71 Roughing

  • Troubleshooting G71 & G72 Roughing Cycles

  •  (Links to an external site.)

• Rules for External Profiling:

  • Make sure the P & Q block lines numbers are unique!  

  • Starting point Z and Point A Z must be same value.

  • Starting point X must be be larger than profile X values.

  • Changing directions only permitted along one axis

Example:

This is typically followed by a G70 for finish stock removal using the same P & Q blocks defining the profile

G96 S1000 (Faster CSS for finish)

G70 P210 Q240 F0.005 (Lower feed rate for finish pass)

Drilling

G83 Peck Drilling 

See Drilling under Feed & Speeds

Video: Haas Tip of the Day - Drilling on a Haas Lathe