How to Run a CNC Program

• 1
  Key takeaways
• 2
  Reading the program and setup sheet together
• 3
  Setting work offsets and tool lengths without guesswork
• 4
  Using dry run and distance-to-go to catch mistakes
• 5
  Running the first part and proving the setup
• 6
  How to run a CNC program: 7 steps from load to first article
• 7
  What to check, what goes wrong, and how to correct it

Before you press anything, compare the program header to the setup sheet. The header usually holds the program number, the part revision, the work offset calls such as G54 through G59, and the tool list. If the revision letter on the screen does not match the drawing in your hand, stop there. Running the wrong revision is one of the few mistakes that cannot be corrected after the fact.

Check the units line next. G20 is inch, G21 is metric. A program written in millimeters and run in inch mode moves 25.4 times farther than intended. The error shows up at the first rapid move, which is exactly when you have the least time to react. Confirm G17 plane selection as well; a wrong plane turns an arc into a straight line or triggers an alarm.

Walk the tool list against the physical carousel. Count the pockets and confirm each tool number matches the holder in that pocket. On a 16-station turret, one tool loaded two pockets out will cut with the wrong geometry and the offsets will not save you. If the shop uses pre-set tooling with measured lengths, confirm those numbers are already in the offset table.

Finally, look at the workholding callouts. The sheet should state the vise jaw position, the stop location, and the minimum clamp height. A part sitting 3 mm above the parallels will move under a roughing pass. Check that the stock sits flat, that the parallels are clean, and that the part cannot rock when you push down on one corner.

• 1
  Program number and revisionMust match the drawing and setup sheet.
• 2
  Units and planeG20 or G21, and G17 for XY arcs.
• 3
  Tool listConfirm pocket position and pre-set length values.
• 4
  WorkholdingClean parallels, flat seating, no rocking.

Work offsets define where the part is in the machine. Touch off X and Y on a machined surface or a known datum, then record the values in the correct offset page. For a vise setup, X is often the fixed jaw and Y is the stop face. Write the numbers down before you move the axes; a jog in the wrong direction after touching off will cost you the reference.

Z is the one that hurts. Touch the tool to the top of the stock with a 0.1 mm feeler or a gauge block, then subtract the gauge thickness from the recorded value. If you touch off with a 50 mm gauge block, the Z offset must be 50 mm lower than the contact point. Operators who forget this step bury the tool in the vise on the first rapid.

Tool length offsets come from a pre-setter or from touching each tool to a common reference. Pre-set values are only valid if the holder is seated the same way in the spindle every time. Wipe the taper and the flange face before loading. A chip between the flange and the spindle face changes the tool length by more than the tolerance you are trying to hold.

After all offsets are set, call each tool in MDI and bring it to a safe Z height above the part. Watch the machine position display, not the tool tip. The display is the only number the control actually trusts. If the displayed Z does not match your arithmetic, re-check the offset before running any part of the program.

• 1
  Gauge block correctionSubtract the block thickness from the Z reading.
• 2
  Clean tapersWipe the holder before every load.
• 3
  Trust the displayVerify Z on screen before cycle start.

Most modern controls offer a graphic simulation and a distance-to-go readout. Use both. The graphic shows the path shape; distance-to-go shows the remaining travel on each axis at any moment. If the Z remaining value suddenly drops to a small number while the tool is still above the part, the program is about to plunge. Hit feed hold and check the block ahead.

Dry run raises the tool by a known amount, usually set in the dry run parameter, and runs the program at rapid. Set the raise value large enough to clear the tallest feature plus the longest tool, typically 50 to 100 mm. Run with rapid override at 25% for the first pass. The point is not to finish quickly; it is to see every move before it happens.

Watch the tool change positions especially. The Z retract height before a tool change must clear the part, the vise, and any clamps. On a 4,000 mm travel machine with tall fixtures, that clearance number can be much larger than the default. If the program retracts to a machine Z that is too low, the tool will drag across the workpiece on its way to the carousel.

Distance-to-go also helps with deep pockets and long tools. A 6 mm end mill at 4× diameter depth will deflect. If the readout shows a full-depth cut in one pass, split it in the program or adjust the depth of cut before running. Dry run does not simulate cutting forces, so use it for geometry and clearance, not for chatter.

• 1
  Set the raise value50–100 mm above the tallest feature.
• 2
  Rapid overrideKeep it at 25% for the first dry run.
• 3
  Check retract heightsMust clear part, vise and clamps.

Switch to single block and run the first tool through its approach and first cut. Listen to the cut. A light, steady sound means the feed and speed are close. A high-pitched squeal means the tool is rubbing; reduce the feed or increase the speed. A dull thud means the tool is overloaded; reduce the depth of cut before continuing.

After the first feature is cut, stop the program and measure it. Do not wait until the part is finished. If the width is 0.05 mm oversize, correct the cutter compensation or the work offset now, while the error is still one feature deep. Measuring at the end, when the part is out of tolerance in six places, gives you no useful direction.

For a ±0.005 mm tolerance, the first-article measurement needs a controlled environment and a calibrated instrument. A micrometer held in a warm hand reads differently than one on a stand. Let the part cool, wipe it clean, and measure at the same temperature as the inspection room. Record the actual value, not just pass or fail.

Once the first part is in tolerance, run the second part without touching the offsets. If it repeats, the setup is stable. If it drifts, the cause is usually thermal growth or a loose clamp. Check the clamp torque and let the spindle warm up for 10 to 15 minutes before judging the result. A machine that has been sitting cold will move as it heats.

• 1
  Single block the first toolConfirm approach and first cut before full run.
• 2
  Measure earlyCorrect the offset after the first feature.
• 3
  Control the temperatureCool part, calibrated instrument, stable room.