📷 IMAGE AREA — Cycle Start, Feed Hold and Emergency Stop keys on a FANUC operator panel
Suggested alt text: Program start pause and emergency stop keys on a FANUC CNC milling operator panel
On a CNC mill, writing the program is not the end of the job; the program must be checked safely before it is applied to a real part. The most important task of a beginner operator is to check the tool path step by step rather than running the program at full speed immediately. In this lesson we learn how to select the program on a FANUC-controlled vertical machining center, how to try it safely, how to check the first part, and how to act when an alarm occurs.
1. Objectives of the lesson
By the end of this lesson the student will be able to distinguish the basic operating modes; select and run a program; understand the roles of the Cycle Start, Feed Hold and Reset keys; check the program line by line with Single Block; use Rapid Override and Feed Override; understand the basic logic of Dry Run and Machine Lock; machine the first part in a controlled way; read the basic information on the alarm screen; and apply the safe action sequence after an alarm.
2. Basic operating modes
Mode names may vary slightly by machine. The most common modes: EDIT — the program writing/editing mode (a program is opened, a line added, a wrong value corrected; the program is not run). MDI — the mode where short commands are entered by hand and run once (e.g. S500 M03; or T01 M06;); the commands are usually not permanent. JOG — manually moving the axes with direction keys (the axis and direction must be checked before moving). HANDLE — fine axis movement with the handwheel; steps ×1, ×10, ×100; with ×100 a small turn creates a large move, so a low step is used near the part. AUTO/MEMORY — the mode where the program in memory is run; after selecting the program, automatic operation starts with Cycle Start.
3. Points to check before running the program
Before pressing Cycle Start, just looking at the program lines is not enough. Check together: is the correct program selected; is the workpiece clamped correctly; are the vise/fixture secure; is the G54–G59 zero correct; are the tool numbers, H length offsets and D radius offsets correct; does the program start with G90; is the safe Z sufficient; are the spindle rpm and rotation direction correct; are the hole depths correct; are G80, G40 and the necessary cancels present at the end? FANUC manuals require checking the entered data, feed values and compensation amounts before actual machining.
4. Selecting the program
General sequence: the mode switch is set to EDIT (or program search) → the program screen is opened → the program number to run is searched → the program’s name and first lines are checked → the mode switch is set to AUTO/MEMORY → it is verified to be at the program start → Single Block and low override are prepared → Cycle Start. The key sequence varies by control model; exact usage follows the manufacturer’s manual.
5. Cycle Start
Cycle Start starts the selected program or resumes a paused program. To run, generally the correct mode must be selected, the door closed, no alarm present, the emergency stop released and the machine in a ready state. With Single Block on, Cycle Start is pressed again for each program line. The FANUC manual explains that automatic operation begins with Cycle Start and can be paused/stopped with Feed Hold or Reset.
6. Feed Hold
Feed Hold pauses the axis feed in a controlled way. It is used to examine the tool path, stop an unexpected move, observe chip formation, or hold the program for a dimensional check. After Feed Hold the program does not end completely; after checking the proper conditions it resumes with Cycle Start. But if a manual move is made while the tool is inside the part, the tool path may change when the program restarts; so operation must not be continued directly after manual intervention.
7. Reset and Emergency Stop
The Reset key can stop the running program and reset some modal operations; but it does not clear every alarm, does not fix a faulty program, and does not replace emergency stop. Emergency Stop is used in a real danger: if the tool is heading fast toward the vise, the part is coming out of the clamping, the tool has broken and a dangerous move has occurred, or the machine behaves out of control. After emergency stop: motion is fully stopped, the cause of the danger is determined, the tool and part positions are checked, the program line is examined, authorized help is obtained if needed, and the program is not restarted until the cause is found.
8. Single Block
Single Block runs each block of the program one at a time. For example in the program below, with Single Block on, Cycle Start is pressed, N10 runs and the machine stops; the next line is checked, Cycle Start is pressed again, N20 runs and the machine stops again.
N10 G00 X20. Y20.;
N20 G43 H01 Z50.;
N30 G00 Z5.;
N40 G01 Z-2. F100.;This method is very useful especially in new programs, newly clamped parts, the first tool approach, G41–G42 entries and drilling cycles. The FANUC manual shows that with Single Block on, one operation block is executed on each Cycle Start press and then the machine stops.
9. Rapid Override and Feed Override
Rapid Override reduces the speed of G00 rapid moves (0%, 25%, 50%, 100%). On the first run of a new program a low value is selected; it matters especially in G00 X... Y...;, G00 Z...; and G43 H... Z...; lines. Rapid Override does not correct a wrong coordinate; it only slows the move to give more control time. Feed Override changes the feed rate of G01/G02/G03 and drilling cycles as a percentage; for example with F300 written, selecting 50% gives an actual feed of ~150 mm/min. A low percentage can be used during the first cut; but constantly lowering the feed too much can make the tool rub instead of cut.
10. Dry Run
Dry Run is a test feature used to try the program’s moves. In this feature the tool motion speed may differ from the normal F value in the program; the panel test/jog speed may take effect. Therefore Dry Run does not always mean slow operation — the FANUC manual states the Dry Run speed can differ from the programmed feed and in some cases be higher. When using Dry Run, keep the tool away from the part if possible, check the clamping, keep Rapid Override low, use Single Block on, and watch the tool path both on screen and physically.
11. Machine Lock and Auxiliary Function Lock
With Machine Lock on, the program can run but the axes do not physically move; the position values may change on screen. It is used to check the general flow of the program. Risks: a difference can arise between the on-screen positions and the real axis position; do not switch to real machining without re-checking the coordinate system. After Machine Lock is turned off, do not give Cycle Start directly; the machine’s real position and the workpiece coordinate must be re-verified. With Auxiliary Function Lock on, spindle rotation, tool change, coolant and some M/S/T commands may not run; used with Machine Lock, the program flow can be watched without movement and auxiliary functions running.
12. Safe program-trial sequence
Basic check sequence for a new program: examine the program line by line on screen; check the tools and offsets; check the workpiece zero; look at the tool path if a program graphic exists; if needed check the flow with Machine Lock and then re-verify the real position; turn on Single Block; lower the Rapid and Feed Override values; run the first tool moves at a safe height; check that the tool goes toward the G54 X0 Y0 point; check the correct H number in the G43 H line; approach the tool to the surface in steps; watch the first cut at low feed; repeat the same checks after every tool change.
13. Machining the first part
The first part is the one on which the program and machine setup are verified. Its aim is not only to finish the part but to check: is the tool cutting in the right place; are the holes in the right position; are the depths and outer/inner dimensions correct; is the surface quality sufficient; is the tool vibrating; is chip evacuation clean; is the spindle load normal; is there movement in the clamping? On the first part, safety and accuracy matter more than speed.
14. Measuring the first part
After machining is complete the part must be measured against the drawing. Tools that can be used: caliper, micrometer, dial indicator, height gauge, bore gauge, gauge block, surface roughness device. When measuring, the part and measuring tool must be clean, the part temperature considered, burrs removed, the measurement taken from the correct surface, and the tolerance on the drawing checked.
15. What to do on a dimensional error?
When the part dimension comes out wrong, the program coordinates must not be changed immediately. First the source of the error is investigated: is the tool worn; is the H length offset correct; is the D radius offset correct; has the G54 zero shifted; has the part moved in the clamping; does the tool have runout; was the wrong tool used; was the drawing misread; was the measurement done correctly? If the main geometry is correct, small dimensional corrections can be made from the Wear offset.
16. Wear offset correction
The Wear field is used for small tool-wear corrections. For example if a surface is left 0.02 mm high, a small correction in the tool length Wear value may be needed; if there is an error in an outer/inner dimension, the D Wear value can be used. But the sign direction must not be entered from memory; ask: should the tool remove more or less material? Large values must not be entered in the Wear field; if there is a large error, the tool, G54, Geometry offset or program must be re-checked.
17. What is an alarm?
An alarm is a message showing that the CNC control has detected a problem preventing normal operation. It can occur due to: a wrong G code, a missing address, a geometric program error, exceeding an axis limit, wrong cycle usage, a tool magazine problem, the door/safety system, a spindle problem, a servo/drive fault, low air or oil pressure, or the emergency stop being pressed. An alarm is not cleared just by pressing Reset; the cause must be understood first.
18. What information is on the alarm screen?
The alarm screen generally shows the alarm number, alarm message, alarm type, program number and the stopped sequence number/block. Example: PS Alarm, Alarm No 010, Message “Improper G-Code”, Program O1001, Block N80. In this example the first place to check is line N80 in the program. The FANUC 0i Model D manual states that there are separate display sections for the alarm screen and the alarm history.
19. Sequence to apply when an alarm occurs
- Check that the machine motion has stopped; read the alarm number and message.
- Find the stopped program line; check the physical condition of the tool and part.
- Determine whether the alarm is program-, operator- or machine-related; look at the alarm description in the manual if needed.
- Correct the cause of the error; verify the tool is in a safe position.
- Restart the program from a safe line; watch the first moves with Single Block and low override.
20. Basic checks on program alarms
On a program alarm, check: is the G code correct; is there a number next to the address; is the decimal point correct; is the G02/G03 arc geometry correct; is the G41/G42 entry move sufficient; is the G81–G84 cycle cancelled with G80; is the G90/G91 state correct; was the wrong plane selected; is there a missing X, Y, Z, R, I, J or K in the program line? When editing the program, a line must not be added randomly in the middle of the running program. The FANUC manual states that continuing from the same place after editing a stopped program can lead to unexpected machine movement.
21. Restarting from the middle of the program
Starting from the middle of the program is risky, because information activated in earlier lines can be skipped (G54, G90, G17, G43 H, G41/G42, spindle rpm, M03, M08, F feed, drilling cycle data). So it is not correct to just find the line to go to and press Cycle Start. The safer method: stop the program with Reset; retract the tool to a safe area; find the start of the relevant tool section; check the tool number, G54/G90/G17 and other modal codes, the H and D offsets, the spindle and coolant; run the tool section from the beginning with Single Block.
22. Continuing after manual intervention
If the tool is moved with JOG or HANDLE after Feed Hold, the relationship between the program position and the real position can change. FANUC safety notes state that after manual intervention, before restarting the program, the manual absolute setting, the G90/G91 state, the coordinate system and the tool path must be checked. A beginner operator must not give Cycle Start directly after manual intervention.
23. Screens to watch while the program runs
The Program screen shows the running line and the next commands. Absolute Position shows the position relative to the active workpiece coordinate; Machine Position shows the position relative to the machine coordinate. Distance to Go shows the remaining move distance in the active block; for example if Distance to Go Z = −25.000 is shown on the Z axis, the tool will move another 25 mm in this block. The Alarm screen shows the active alarm and message.
24. First-part checklist
Before the program starts: the correct program is selected; the correct tool is loaded in the magazine; the T and H numbers match; the D offset is correct; G54–G59 are correct; the part is firmly clamped; the safe Z is sufficient; Single Block is on; Rapid and Feed Override are low; the door is closed; the emergency stop location is known. During machining: the tool moves in the correct direction; the tool is away from clamping elements; the cutting sound is normal; chip evacuation is clean; the spindle load is normal; the coolant works correctly. After machining: the part is measured; burrs are checked; the surface quality is examined; the required Wear correction is recorded; tool wear is checked.
25. Shutting down the machine safely
The shutdown sequence varies by machine builder; the general logic: the program is fully stopped → the spindle is stopped → the coolant is turned off → the tool and axes are moved to a safe position → the large chips on the table and work area are cleaned → a reference/park position is used if necessary → the control is turned off with the proper Power Off key → the main switch is turned off per the builder’s procedure. The emergency stop button must not be used like a normal daily shutdown switch; the real shutdown procedure must follow the builder’s manual.
26. What we learned throughout the basic series
By the end of these nine lessons the student has learned the basic structure of the CNC mill; the X, Y and Z axes; the workpiece coordinates; G90 and G91 programming; the FANUC program structure; the G00, G01, G02 and G03 moves; cutting tool selection; the logic of speed and feed; workpiece clamping and zeroing; G43 tool length compensation; G40, G41 and G42 radius compensation; the G81, G82, G83 and G84 drilling cycles; safely checking the program; machining the first part; and reading the basic alarm screen. This level does not mean the student is authorized to work alone on a real machine; but it provides a solid start for CNC milling training and supervised shop practice.
📷 IMAGE AREA — Alarm screen: alarm number, message and stopped block; the first-part check flow
Suggested alt text: Alarm number message and program line on a CNC milling alarm screen with the first-part check flow