How to Make a CNC Machine Reset Bit Position Z Axis

• 1
  Key takeaways
• 2
  Pre-Reset Checks That Save a Second Setup
• 3
  How Machine Type Changes the Reset Bit Position Z Axis Procedure
• 4
  Choosing a Touch-Off Method and Reading the Result
• 5
  When the Z Axis Will Not Hold After a Reset
• 6
  Step-by-Step: Reset Bit Position Z Axis
• 7
  Reset Method and Verification by Machine Type

Most failed resets are not control problems. They are mechanical. Before you open the offset page, stop the spindle, remove the tool, and check the holder taper and pull stud for fretting or chips. A collet that has been over-torqued will pull the tool 0.01–0.03 mm deeper on the next clamp, and no amount of re-touching will hold.

Wipe the spindle nose and the tool taper with a lint-free cloth. Check runout with a dial indicator at 25 mm from the holder face. On a healthy CAT40 or HSK-A63 holder, runout should stay under 0.010 mm. If it reads 0.03 mm or more, swap the holder before you reset bit position z axis.

Confirm the machine is in the right mode. Reference return on most Fanuc and Siemens controls requires the Z axis to be at least 20 mm above the soft limit before you press the zero-return key. Pressing it from the bottom of travel trips an overtravel alarm and forces a manual jog-out.

Write down three numbers before you change anything: the current work offset Z, the tool length offset for the tool in the spindle, and the machine coordinate reading at the reference point. These three values tell you later whether the reset moved the zero point or the tool data. Without them, you are guessing.

• 1
  Holder conditionTaper clean, pull stud torqued to spec, runout under 0.010 mm at 25 mm.
• 2
  Axis positionZ parked at least 20 mm above the soft limit before reference return.
• 3
  Recorded valuesOld work offset Z, old tool length offset, machine Z at reference.
• 4
  Stock and fixtureTop face clean, no burr, no coolant film where the tool will touch.

On a 3-axis vertical mill, Z reference is simple. Home the machine, load the tool, jog down until the tip touches your reference surface, and enter the difference into the work offset or the tool length offset. The choice matters. If one tool is wrong, edit the tool length. If every tool is off by the same amount, edit the work offset. Mixing the two is how a shop ends up with one tool cutting 0.5 mm deep.

A 4-axis machine adds a rotary table, so the Z reference depends on where the part sits relative to the rotary centerline. After any change to the chuck, tombstone or fixture plate, re-measure the centerline height and update the rotary offset before you touch off. If you skip this, the Z value will be correct at A0 and wrong at A90, which usually shows up as a taper on the side of the part.

Simultaneous 5-axis work is stricter. With two rotary axes in motion, the tool tip position depends on the kinematic model, not just a single Z number. After a crash or a spindle change, run a probing cycle on a known sphere or gauge block and let the control rebuild the tool center point. Hand-entering a Z offset on a 5-axis machine without re-checking the kinematic chain is a reliable way to scrap an expensive part.

The table below shows the tolerance band we hold after a reset on each machine class. These are shop floor numbers from our own cells, not machine specs.

• 1
  3-axisWork offset or tool length edit, verify within 0.01 mm.
• 2
  4-axisRe-check rotary centerline height first, then touch off.
• 3
  5-axisRe-probe the kinematic model, do not hand-edit Z alone.

A 0.01 mm dial or digital gauge on a magnetic base is still the fastest way to touch off a single tool on a 3-axis machine. Bring the tip down in 0.1 mm steps until the needle moves, then back off and approach in 0.01 mm steps. The reading where the needle first moves is your Z0. Repeat it twice. If the two readings differ by more than 0.005 mm, something is loose.

A spindle probe is faster and removes operator feel from the loop. Most probe cycles touch the surface twice and average the result. Watch the spread between the two touches on the control screen. A spread above 0.008 mm usually means chips on the surface or a dirty stylus, not a bad probe.

A paper slip or feeler gauge is acceptable for rough work only. Paper compresses and the thickness varies by 0.02–0.05 mm depending on humidity and grade. If the drawing calls for ±0.05 mm on a depth, that error eats most of your budget.

After any method, cut a test feature. Face a scrap plate 0.2 mm deep and measure the step with a micrometer. If the measured depth matches the commanded depth within 0.01 mm, the whole chain from offset to servo is good. If it is off by a consistent amount, the error is in the offset. If it varies across the plate, the problem is mechanical, not the reset.

• 1
  Gauge + indicatorBest for single tools, repeat twice, accept under 0.005 mm spread.
• 2
  Spindle probeFast, watch the two-touch spread, clean the surface first.
• 3
  Paper or feelerRough work only, expect 0.02–0.05 mm uncertainty.
• 4
  Test cutFace 0.2 mm on scrap, verify within 0.01 mm before running the job.

If Z drifts after a correct reset, separate thermal growth from mechanical slip. Run the spindle at your normal cutting speed for 30 minutes, then re-touch the same tool on the same surface. A shift of 0.01–0.02 mm over that period is normal thermal growth on many machines. A shift of 0.05 mm or more points to a mechanical fault.

Check the tool clamp first. A weak Belleville stack or a worn drawbar lets the tool creep under load. Pull the holder and inspect the taper for a bright wear band near the flange. A uniform contact pattern is good. A narrow shiny ring means the taper is not seating, and the tool will move in Z whenever the load changes.

Ball screw backlash and thrust bearing play show up as a difference between approaching Z0 from above and from below. Touch off from +0.5 mm, record it, retract, and approach from -0.5 mm. If the two values differ by more than 0.01 mm, the axis has backlash that needs mechanical attention, not another offset edit.

A hard crash can bend the ball screw or shift the coupling. After a crash, re-reference the machine and check the Z repeatability at three heights: near the top of travel, mid-travel, and 50 mm above the table. Any height that reads outside 0.01 mm needs a service call before you run production.

• 1
  Thermal growth0.01–0.02 mm after 30 minutes at cutting speed is normal.
• 2
  Tool creepWorn drawbar or Belleville stack, look for a narrow contact band.
• 3
  BacklashCompare approach from above and below, over 0.01 mm is a fault.
• 4
  Post-crashCheck repeatability at three heights, not one.