Program Loading, Review, and Dry-Run Prove-Out

Why Prove-Out Matters

Every new or revised NC program must be proven safe before the cutter touches metal. A single incorrect coordinate, a missing tool call, or a wrong work offset can drive a tool into a vise jaw, break a spindle, or injure the operator. The prove-out sequence — file transfer, code review, and dry run — gives you three separate chances to catch errors before damage occurs. This lesson covers all three steps as performed on a Haas CNC mill.

Step 1: Transferring the Program

USB transfer is the simplest method. Insert a FAT32-formatted USB flash drive into the Haas control's front USB port. On the control, navigate to LIST PROGRAMS, select the USB device, highlight the file, and press SEND TO MEMORY. The control copies the file into its internal program memory and assigns it a program number (O-word). Before moving on, compare the file size and line count displayed on the control against the values on the source computer. A mismatch means the transfer was incomplete or the wrong file was selected.

DNC (Direct Numerical Control) streams the program from a PC to the control in real time through a network or serial connection rather than storing the whole file first. This is common for very large programs that exceed control memory. The instructor PC runs DNC software; the Haas is placed in DNC or Remote mode. After transfer, confirm line count and file size the same way you did for USB.

Always verify both transfer methods produce identical results. If they differ, do not proceed.

Step 2: Program Code Review

Print the program and use the program-review checklist to scan it line by line. You are looking for errors that software post-processors and CAM systems can introduce. Work through the checklist in order:

1. O-word / program number — present and matching the job traveler.

2. Safety block — typically G17 G20 (or G21) G40 G49 G80 G90 at the top to cancel cutter comp, tool-length offset, canned cycles, and set modal defaults.

3. Tool calls (T-word) — every tool used must be called before it is used.

4. M06 (tool change) — each T-word must be followed by an M06; a missing M06 means the spindle tries to cut with the wrong tool.

5. Work offset (G54–G59 or G54.1 Pn) — must appear before the first motion command for each setup.

6. Spindle speed (S-word) and direction (M03/M04) — must appear before the tool reaches the part.

7. Feed rate (F-word) — every cutting move must have a feed rate; rapid moves (G00) do not require F, but the first G01/G02/G03 must.

8. Canned cycle cancel (G80) — must appear after all hole operations before other motion.

9. Program end (M30 or M02) — missing end causes the control to fault or run into empty memory.

10. Unclosed loops (M98/M99 subprogram calls) — every call to a subprogram must have a matching return; count them.

Annotate every finding directly on the printed copy with a red pen. Record each finding on the checklist form with the line number and a brief description.

Step 3: Dry Run with Raised Z and Feed-Rate Override

The dry run proves tool path geometry without cutting metal. Two protections work together:

• Z raised 2.000 inches: In the work offset table (G54 or the offset in use), add +2.000 in to the Z value, or use the OFFSET page to shift Z up by 2.000 in. This lifts every programmed Z position by two inches so the tool moves through air where the part surface would be. The 2.000 in margin gives clearance above a typical workpiece and vise jaw while still letting you observe realistic X–Y motion.
• Feed-rate override at 5%: Turn the feed-rate override (FRO) dial to 5%. At 5% of programmed feed, motion is slow enough to observe and react before a bad move reaches the part or fixture. Rapid moves are also slowed by the rapid override; set rapid override to 25% or 5% per shop practice.

Single-block mode (SINGLE BLOCK button on the control) executes one block at a time. After each block executes, the machine stops and waits for you to press CYCLE START again. This lets you monitor each motion individually and compare it to the Haas graphics display before committing to the next move.

Haas graphics mode shows a 2-D or 3-D preview of the tool path. Run the program in GRAPHICS before the dry run to verify the path looks correct on screen, then switch to single-block dry run for the physical prove-out.

During the dry run, watch for:

• Unexpected rapid moves toward the part or fixture
• Wrong plane (G17/G18/G19) causing arc motion in the wrong axis
• Tool-length compensation not active (G43 missing) causing Z to be unpredictably low
• Any machine alarm — stop, investigate, and correct before continuing

If the tool moves toward the work unexpectedly, press FEED HOLD immediately, then RESET. Do not attempt to catch or redirect the machine.

Lockout/Tagout and PPE

LOTO is not applied during prove-out because the machine must run. Instead, apply these controls:

• Safety glasses at all times in the machine area.
• Keep the machine guard door closed during spindle-on phases. Open only when the spindle is fully stopped.
• No loose clothing, gloves, or jewelry near rotating parts.
• One operator at the control at a time; a second person may observe but must stand clear of the machine envelope.
• Know the location of the E-stop before you start CYCLE START.

Completing Prove-Out

The dry run is successful when the program runs to M30 without a machine alarm and without the tool contacting the 2-inch air-cut reference plane. After a successful dry run, restore the Z offset to its correct (un-shifted) value, reset the FRO to 100%, and obtain instructor sign-off before cutting the first part.