INTRODUCTION:
When you first stand in front of a Vertical Machining Center (VMC), the mode selector switch is your primary way of telling the machine exactly how you want it to behave at any given moment. Think of it like a gear shifter or a set of driving modes in a car each position changes the machine's response to your inputs, keeping you safe and in control. Let's walk through them in a logical order.
EDIT mode is where you write or modify the G‑code program. The machine will not move at all here, so you can safely type, delete, or rearrange lines of code without any risk of unexpected motion. JOG mode lets you move an axis continuously while you hold down a button typically at a faster feed rate which is perfect for rough positioning, like moving the table out of the way to load a part. HANDLE mode (sometimes called MPG or handwheel mode) gives you a rotating wheel; each click moves the axis by a tiny, precise increment, such as 0.001 inch or 0.01 mm. This is what you'll use for careful tasks like touching off tools, finding part edges, or sneaking up on a zero point.
REFERENCE mode (often labeled REF or HOME) is non‑negotiable: it's the first thing you should do after powering up the machine. It forces each axis to travel until it finds its grid zero, establishing a known starting point for all subsequent moves. Without referencing, the machine has no idea where it is, and that can lead to crashes. MDI (Manual Data Input) mode allows you to type a single line of G‑code for example, S500 M03 to start the spindle at 500 RPM and then press cycle start to execute just that one command. It's incredibly useful for quick tests, tool changes, or moving to a specific coordinate without running the full program. Finally, AUTO mode is the "full robot" state: once you've selected your program, pressing cycle start runs it from beginning to end, automatically executing every command. This is what you use for actual cutting of parts, but you should only switch to AUTO after you've proven the program in a safer mode like single‑block or with the feed override turned way down.
A good rule of thumb for beginners: spend your early hours getting comfortable in HANDLE and MDI, because those give you direct control with very low risk. Save AUTO for when you have double‑checked everything your tool offsets, work offset, and the distance‑to‑go display. Think of the mode switch as your permission system: it's not just a selector, it's a safety device.
AUTO Mode:
In a VMC, AUTO mode is the absolute core of production. It stands for Automatic execution, meaning the machine controller takes full control of the physical axes, spindle, and tool changer to execute a stored CNC program from start to finish without human intervention.Why We Use AUTO Mode?
Humans cannot move three axes simultaneously with the perfect, synchronized precision required to cut complex shapes. AUTO mode ensures that the 1st part and the 100th part are identical down to microns. A VMC running in AUTO mode utilizes optimized feed rates (G01, G02, G03) and rapid movements (G00) that are impossible to duplicate manually. It reduces cycle time to the bare minimum. For advanced toolpaths generated by CAM software like PowerMill, the code contains thousands of tiny coordinate lines. AUTO mode is the only way the controller can process these complex paths smoothly. It allows one operator to manage multiple machines simultaneously. Once AUTO mode is active, the operator's job shifts to monitoring tool wear and reloading raw material.
How to Use AUTO Mode:
Running a machine in AUTO mode can be dangerous if steps are skipped. In EDIT mode, select or upload the correct program number (e.g., O1234) into the machine memory. Ensure your work coordinate offsets (G54) and tool length offsets (G43) are correctly set and verified.
Turn the mode selection dial to AUTO or MEM. Never just press cycle start on a fresh program at 100% speed. You must prove it out to avoid a costly crash.
Turn on Single Block (SBK), this forces the machine to stop after every single line of code. Turn the Feedrate Override and Rapid Override (G00) down to 0% or 25%. Press the Cycle Start button. Keep your hand firmly on the Feed Hold button.
Look at your controller screen to check the "Distance-to-Go" display as the tool approaches the raw material to ensure it doesn't plunge too deep. Once the first tool successfully finishes its cut and you see the code is correct, turn Single Block OFF. Turn your overrides up to 100%.
Let the machine run automatically until it hits an M30 (End of Program) command, which stops the spindle and resets the program to the top.
If you are getting ready to run a program you wrote manually, also preparing to transfer a heavy toolpath out of PowerMill to run in AUTO, so how to do it?
Running a manually written program versus transferring a massive PowerMill CAM file require two slightly different approaches. Because your manual program is small, it can be typed or loaded directly into the machine's internal memory (AUTO/MEM mode). However, because your PowerMill program contains thousands of lines of code for complex toolpaths, it likely won't fit in the machine's internal memory. For that, you will use DNC/RMT mode to run it directly from a USB drive, CF card, or an Ethernet/RS-232 link to your PC.
If you wrote this program manually, the priority is verifying that there are no typos like a missing decimal point or an accidental G00 instead of G01.
Turn the mode dial to EDIT. Press the PROG key on your controller. Type your program number (e.g., O0005) and press the arrow down key, or input it via USB. Carefully scroll through the code on the screen. Look closely at your G, M, X, Y, and Z codes to catch any manual typing mistakes.
Switch to HANDLE/MPG mode. Use an edge finder or dial indicator to find your workpiece zero. Register these coordinates into your G54 work offset page. Touch off your tools to find their lengths, and input those values into the TOOL OFFSET (Length/H) page.
Switch the mode dial to AUTO (or MEM). Press the Single Block (SBK) button to turn it ON. Turn your Dry Run (DRY) switch ON (highly recommended for manual code). Turn your Feedrate Override and Rapid Override dials down to 0%. Press the green Cycle Start button. The machine will read just the first line and stop. Gradually increase the rapid override dial to 25%. Press Cycle Start line-by-line.
Always keep one hand on the Feed Hold button or Emergency Stop and keep your eyes on the Distance-to-Go (Dist-To-Go) screen. If the screen says the tool has 50 mm left to go in the Z-axis, but the tool is already touching the job, press Feed Hold immediately.
Once you have stepped through the code safely and confirmed the toolpath looks correct, turn Single Block OFF, turn Dry Run OFF, set your overrides to 100%, and let the machine run automatically to the end (M30).
How to deal with complex 3D toolpaths from PowerMill, the file size is too massive for standard machine memory?
In PowerMill, ensure your toolpath is completely calculated. Right-click on the NC Program and select Write. Ensure you are using the correct Post-Processor file that matches your machine's controller. This will generate a .NC or .TXT file on your computer depending on how your workshop is set up, save the post-processed file using one of these following method.
If you are saving in USB Flash Drive / CF Card, save the file directly onto the card. Ensure the file name is simple, like O1000.NC or TEST.TAP, depending on what your controller prefers. If you use a cable linking your PC to the machine, open your DNC transfer software like Cimco Edit and queue the file up for transmission.
Now setup machine in Remote mode. Plug your USB or CF card into the machine panel. Turn the mode dial to RMT (Remote) or DNC mode. On some Fanuc controllers, you select MEM mode, press the PROG hard key, select the Device soft key to view the USB/Card, and select DNC-ST or DNC-CD. Select your PowerMill file from the list. The screen should now show the first few lines of your PowerMill code, but a "DNC" or "RMT" status indicator will flash on the screen, showing it is ready to stream.
Because PowerMill toolpaths involve thousands of rapid movements, do not use Dry Run as it can cause the machine to ignore programmed feed rates, which is dangerous for 3D paths.
Turn Single Block ON. Turn Rapid Override to 25% or lower. Press Cycle Start. Step through the first few lines of code where the tool moves from the tool changer down toward the part. Once the tool safely reaches its initial cutting depth and begins its first machining pass, turn Single Block OFF and let the DNC stream the heavy toolpath smoothly from your media source.
EDIT Mode:
EDIT Mode is the control center for managing your CNC programs. Unlike AUTO mode which executes code or MANUAL modes which move the physical axes, EDIT mode disconnects the machine’s physical axes and opens up the controller's internal storage drive.
How to Use EDIT Mode Step-by-Step?
Activate the EDIT mode by turning the mode selection dial to EDIT. Press the PROG (Program) function key on the keypad to display the program text on the screen. To open an existing program, type the letter O followed by the program number (e.g., O1002) and press the Arrow Down key or the O-SRCH (Program Search) softkey. To create a blank program, type a new, unused program number (e.g., O5555) and press the INSERT key.Once your cursor is on the line of code you want to change, you use following three primary keys:
ALTER: It replaces an existing code. e.g. Move cursor to S1200, type S1500, and press ALTER to update the speed.
INSERT: It adds new code directly after the cursor. e.g. Type M08 and press INSERT to add coolant.
DELETE: Removes the word or block where the cursor is currently flashing.
Your every line of manual G-code on a Fanuc-style controller must end with an End-of-Block character. Always press the EOB key which inputs a semicolon " ; " before pressing INSERT.
Why We Use EDIT Mode?
We can write short, simple programs from scratch directly on the machine console, e.g., facing a raw block, cutting a simple rectangular pocket, or drilling a basic bolt hole pattern. The operator creates a new O number and manually types line-by-line (G90 G54 G00 X0 Y0...) using the alphanumeric keypad to build the entire program.Adjusting cutting parameters after reviewing the first machined part or during a live test run. If you notice a tool vibrating (chattering) or cutting too slowly, you switch to EDIT mode to locate that tool section and lower the feed rate (F) or adjust the spindle speed (S). You can also add an optional stop (M00 or M01) before a critical tool path so you can measure the part mid-operation.
You don't have to go back to your PC and CAM software every time you need to change a simple feed rate, spindle speed, or tool number. You can fix it right at the machine console. While in EDIT mode, the machine’s spindle and axes are completely locked out from moving. Even if someone accidentally presses the green "Cycle Start" button, the machine will not move.
Sometimes a PowerMill post-processor outputs an unexpected code that causes the machine to alarm out like an unsupported G or M code, or a missing decimal point like X50 instead of X50.0. You use EDIT mode to find the faulty line and clear or correct the code.
It allows you to manage the controller’s memory—deleting old programs, creating new program numbers, and copying code blocks. While in EDIT mode, you can access the I/O (Input/Output) utilities page. This is where you copy files from a USB flash drive or CF card directly into the machine's internal memory storage.
If your machine throws an alarm during a test run for example, a syntax error or a missing code, EDIT mode is where you go to find that specific line and correct it. If a drill breaks mid-program, or a tool cuts slightly shallow and you need to rerun only that specific tool rather than running the whole program from the beginning. In EDIT mode, you use the search keys to find the specific tool call block (e.g., searching for T05). Once the cursor is placed right at that tool block, you can switch back to AUTO mode to execute the program from that point forward.
MDI Mode:
MDI Mode stands for Manual Data Input. It is a hybrid mode that acts as a bridge between full manual control and full automatic programming.In MDI mode, you can write short lines of G-code or M-code directly on the console screen and execute them instantly. Once you press the green Cycle Start button, the machine runs the commands and then automatically clears or forgets them. It does not save the code into the machine's permanent memory.
Why We Use MDI Mode?
It saves you from having to create, name, and delete a whole program file just to do a 5-second task like turning on the spindle.While manual mode like MPG/Handwheel is great for rough movements, MDI allows you to move the machine to exact mathematical coordinates safely.
It is the primary mode used to verify that specific mechanical features of the VMC are working properly (like checking if the coolant pump works or testing an optional indexer table).
How to Use MDI Mode Step-by-Step?
Here is the standard workflow to input and execute a command safely in MDI.Activate MDI by turning the mode selection dial to MDI. Press the PROG (Program) function key on your keypad. On most modern controllers like Fanuc, this will bring up a blank or short entry screen labeled PROGRAM (MDI).
Type the code by using the alphanumeric keypad to type your commands. Just like in EDIT mode, you must end every command sequence with an End-of-Block character by pressing the EOB key which inserts a semicolon " ; ".
Press the INSERT key to push your typed code onto the active screen area.
e.g. To spin the spindle clockwise at 1500 RPM. Insert this code,
M03 S1500 ;
To execute the program safely, Before pressing the start button, ensure your Feedrate Override or Rapid Override is turned down, especially if you typed a movement command. Ensure the workspace is clear of clamps or tools. Press the green Cycle Start button. The machine will immediately perform the action.
MDI is used constantly throughout the working day by machinists and setup programmers.
We use MDI to command tool change, instead of manually indexing an umbrella or chain tool changer, machinist type: T02 M06; When you press Cycle Start, the machine automatically executes a safe Z-axis retraction, spins the tool carousel to Tool 2, and swaps it into the spindle.
We use it to control Spindle and Coolant.
e.g.
1. To start the spindle: M03 S1200 ; This turns spindle clockwise at 1200 RPM.
2. To stop the spindle: M05 ;
3. To turn on flood coolant: M08 ;
We use it to move the spindle or table to a precise coordinate before finding your work offsets.
e.g.
If you need the table to center exactly on your fixture base, manual jogging might take too long or be inaccurate. You can type: G90 G54 G00 X0 Y0 ; The machine will move rapidly to the absolute center point of your G54 register.
We can activate special machine functions like M-codes by locking/unlocking a 4th-axis rotary table, opening automatic doors, or orienting the spindle.
e.g.
1. To locks the spindle in a precise angular position so the drive keys line up perfectly—critical before loading a boring bar or checking an alignment with a dial indicator
M19 ; (Spindle Orientation: L)
2. To unclamping and clamping a 4th-axis indexer
M11 ; / M10 ;
We use it for quick facing or material flattening. We use it to cleaning up a rough top surface of a raw block before running your main PowerMill program.
e.g.
Rather than generating a CAM path, you can use MDI to make a single manual pass with a large face mill:
G90 G54 G01 X250.0 F500 ; This feeds the tool across the part at exactly 500 mm/min up to the 250 mm coordinate mark.
You do not add a program number like O1234 in MDI mode. When you are in MDI mode, the controller acts like a temporary scratchpad. It does not need a program number because you are not saving a permanent file into the machine's memory—you are just giving it direct, immediate commands.
When you switch your selection dial to MDI and press the PROG hard key, you will notice the screen looks different than it does in EDIT mode. At the top of the screen, the controller will typically display a generic title like PROGRAM (MDI) or O0000. The machine automatically reserves O0000 purely for temporary MDI entries. You cannot rename this or change it to your own program number.
Instead of starting with a program number, you start typing your actual $G$ or $M$ codes immediately.
If you want to quickly change to Tool 2 and start the spindle at 1200 RPM, you simply type:
T02 M06 ;
M03 S1200 ;
Then you press Cycle Start, the machine executes the tool change, spins the spindle, and the lines will either clear out or wait to be overwritten.
JOG Mode:
JOG mode gives you direct, real time control over the physical movement of the X, Y, and Z axes using buttons or switches on the operator panel. As long as you hold down an axis button like +X or -Z, the machine moves. The moment you let go, it stops.
Why We Use JOG Mode?
It is the fastest way to manually clear the spindle away from a finished part or fixture so you have room to clean the table, check surface finishes, or change raw stock.Before you can use a fine handwheel (MPG) to precisely set your work offsets, you use JOG mode to quickly bridge long distances across the machine bed.
If a tool breaks mid-cut or the machine stops unexpectedly, JOG mode allows you to safely back the Z-axis straight up out of the raw material to inspect the damage.
How to Use JOG Mode Step-by-Step?
Because JOG mode moves massive mechanical axes under direct human control, you must pay close attention to your feedrate settings to avoid hitting a clamp or the machine walls.Activate the JOG mode by turn the main mode selection dial to JOG. First we have to set our Jog feedrate. Locate the Jog Feedrate Override dial on your panel usually measured in mm/min or inches/min.
Always start with this dial set low e.g., 100-300 mm/min. If you accidentally press the wrong axis button, a low feedrate gives you enough time to lift your finger before a crash occurs.
Now move the axes by pressing and holding the desired axis direction button on the panel
1. +X / -X (Moves the table left or right)
2. +Y / -Y (Moves the table forward or backward)
3. +Z / -Z (Moves the spindle up or down)
The axis will move continuously at your selected feedrate until you release the button.
Most modern controllers feature a rapid jog modifier button often labeled RAPID or RPD. If you hold down the RAPID button while pressing an axis direction button, the machine ignores your jog dial and moves at its maximum rapid traverse rate (G00 speed). Only use this when the tool is high up and completely clear of all hazards.
JOG mode is used heavily during the setup phase of every single job. When a program completes, the spindle might be sitting near the part. The operator switches to JOG mode, holds down +Z to retract the head safely, and jogs the Y-axis forward so the table moves close to the operator door for easy part loading.
We can use it for rough positioning for work offsets. If the tool changer is at the far back corner of the machine, using a precision handwheel (MPG) to cross the whole bed would take hundreds of rotations. Instead, the machinist uses JOG mode to rapidly drive the axes until the edge finder is hovering roughly 10-20 mm away from the workpiece corner. From there, they switch to HANDLE/MPG mode for the final precise contact.
At the end of a shift, a machinist will switch to JOG mode and drive the table all the way to the far left (-X), wash down the right side with a coolant gun, and then jog it all the way to the right (+X) to clean out the remaining chip chips from the machine enclosure.
We use it during recovery from an Emergency Stop or Power Cut. If the power cuts out or someone hits the E-stop while a face mill is down inside a pocket, the machine memory loses track of its current path. You cannot use AUTO mode to resume. Once power is restored, you must use JOG mode to slowly and carefully lift the Z-axis straight up out of the pocket before doing anything else.
HANDLE (MPG), RAPID, and REFERENCE (HOME):
HANDLE (MPG), RAPID, and REFERENCE (HOME) modes give you complete authority over how the machine moves when it isn’t running an automatic program.
HANDLE Mode (MPG - Manual Pulse Generator):
HANDLE mode is the precision mode of the VMC. It hands over movement control to a physical rotary handwheel called the MPG. Turning the wheel clockwise moves the axis in the positive direction; turning it counterclockwise moves it in the negative direction. It allows you to move the machine axes by increments as tiny as 1 micron (0.001 mm), which is critical for precise setup work where hitting the part too hard will break a tool.
How to Use Handle Mode?
Activate Handle mode by switching the mode selection dial to HANDLE (or MPG). On your pendant or panel, select the specific axis you want to move (X, Y, or Z). Rotate the handwheel slowly to move the axis. Only one axis can move at a time. Select your increment multiplier: 1. x1: Each click/notch of the wheel moves the axis 0.001 mm.
2. x10: Each click moves the axis 0.01 mm
3. x100: Each click moves the axis 0.1 mm
When using an edge finder, you jog roughly close to the part, then switch to HANDLE mode at x10 or x1 to slowly click the wheel until the edge finder kicks sideways, signaling you've found your exact zero coordinate.
Bringing a newly loaded tool down onto a tool setter or a slip gauge resting on top of the workpiece to record the tool's Z-axis length offset.
Manually winding a tool down into a tight pocket or near a fixture clamp to visually confirm that your setup matches your drawing clearances before pressing cycle start.
2. RAPID Mode:
RAPID mode is essentially a high-speed modifier for manual positioning. On some older machines, it is a dedicated position on the mode dial; on most modern controllers, it is activated by holding down a "Rapid Traverse" button while simultaneously pressing a direction button.
Why We Use It?
VMC machine beds can be large (1000 mm). Moving from one extreme end of the table to the other using standard JOG or HANDLE would take way too long. RAPID mode drives the axes at the machine's maximum built-in velocity i.e. G00 speed.
How to Use It?
To activate rapid mode, switch dial to RAPID mode, select your axis button, and press down. If it's a modifier button, stay in JOG mode. Hold down the RAPID modifier button often looks like a running man or a fast arrow symbol and press your axis direction key (+X, -Y, etc.).Shifting the machine table from the far left back to the far right to clear space after a long machining cycle.
After a program finishes or halts, you use RAPID to instantly pull the spindle head straight up to its highest limit so you can safely look inside the machine enclosure without anything blocking your view.
3. REFERENCE Mode (REF / HOME / ZRN):
REFERENCE mode also known as Zero Return or Home mode is used to establish the machine's own coordinate framework. It synchronizes the controller's internal positioning software with the physical, absolute limit switches of the machine.Why We Use It?
When a VMC is powered off, the controller forgets exactly where the table and spindle are sitting. REFERENCE mode sends every axis back to its absolute factory-set limits (Machine Zero) so the controller can accurately locate your G54 coordinates later.How to Use It?
Activate the REFERENCE mode by switching the mode selection dial to REF, HOME, or ZRN (Zero Return). For safety, always home the Z-axis first to pull the tool up and away from anything on the table. Press the +Z button. The head will move up, hit its deceleration switch, slow down, and lock onto its home position. Next, press the +X and +Y or -X/-Y depending on the machine build to send the table back to its home limits.This is always the very first step performed immediately after flipping on the main machine breaker and releasing the emergency stop button in the morning.
On many older or highly rigid VMCs, the automatic tool changer will refuse to execute an M06 command unless the Z-axis is returned to its exact reference home point first.
Programs often end with a G28 G91 Z0 Y0 command, which automatically calls a reference return to move the table all the way forward and the spindle all the way up, making it easy for the operator to clean out chips and swap parts safely.
Changing modes does not change, reset, or alter anything you did in the previous mode.
• If you are in EDIT mode and you type half of a program, then switch to JOG to move the table, your typed code stays exactly as it is. When you switch back to EDIT, your cursor will be flashing on the exact same letter you left it on.• If you move your tool to a corner in HANDLE mode and press X --> ORIGIN to zero out your Relative screen, that zero point is locked. You can switch to MDI, EDIT, or AUTO mode, and the machine will still remember exactly where that relative zero is.
• Your offset tables are permanent registries. Switching modes never changes your offset numbers. The only way those numbers change is if you manually type over them or press the MEASURE key.
There is only one major thing that resets when you switch modes: An active running program. If you are running your program in AUTO (MEM) mode and the machine is mid-cut, the moment you turn the dial away from AUTO like switching to JOG or HANDLE, the machine will instantly feed-hold and stop moving for safety.
If you switch back to AUTO, on most controllers, you cannot just hit Cycle Start to continue from where it stopped. The controller's brain drops the program history, and you will usually have to hit the red RESET button to take the program back to the very top line before you can run it again.
Aside from a running program stopping, everything else—your code, your screen layouts, and your coordinates—stays perfectly untouched!
Your program will stay active on the screen unless,
• You type a new program number: If you type a different number (like O0055) and press the O-SEARCH softkey, the screen will switch to show that other program instead. Your old program is still safe in the memory; it is just hidden from view.
• DELETING: You have to intentionally type your program number (e.g., O0112) and press the DELETE softkey to physically erase it from the machine.
• If you press the red RESET button while looking at the program, it won't delete your text, but it will jump your cursor all the way back to the very top line (O0112).
Here are the critical precautions you must follow to ensure your setups are safe and your machine never crashes.
1. Mode Change Precautions:
This is the most common area for major accidents. If you are running a program in AUTO and need to switch to JOG or HANDLE to check something like a tool tip or a surface finish, follow these rules:• Never turn the mode dial while the machine is actively moving at full feedrate. Press the flashing red FEED HOLD button first, wait for all axis motion to come to a complete stop, and then switch your dial to JOG or HANDLE.
• On some older or heavily worn controllers, switching directly from a high-speed AUTO motion to HANDLE mode can cause a slight electronic delay where the axis "creeps" or drifts a fraction of a millimeter. Always make sure your handwheel multiplier is set to x1 or completely turned off when making the switch so you don't accidentally bump the wheel.
• The Reset Rule: Remember that switching out of AUTO mid-program drops the machine's look-ahead memory. When you switch back to AUTO, do not just press Cycle Start. You must hit RESET to send the program back to the top, or use a safe Block Search to restart from a safe tool-change line (M06).
2. Hard Key Selection Precautions in EDIT & MDI:
When you are tapping buttons on the MDI/EDIT keypad, a single wrong keystroke can alter an entire coordinate system or overwrite code.• Always keep your eyes on BUFFER LINE. When you type letters and numbers on the keypad, they don't immediately go into the machine. They sit at the bottom of the screen in a temporary text line called the Input Buffer. Always read this line with your eyes before you press INSERT, INPUT, or ALTER.
• When you are working on the Offset or Work coordinate pages: INPUT completely erases the old number and overwrites it. +INPUT adds or subtracts your number from the old number. If you mean to adjust a tool wear by -0.02, and you accidentally press INPUT instead of +INPUT, you will wipe out your entire tool length registry, causing a massive crash on the next cycle.
Alway keep a Finger on RESET/Emergency Stop: When executing a newly typed line in MDI mode, keep your left hand hovering directly over the red RESET key or the E-STOP button. If the machine moves in an unexpected direction when you press Cycle Start, hit it instantly.
3. Always check where your cursor is resting:
When you are switching screens using the hard keys like jumping from POS to PROG or OFFSET, the yellow cursor on the screen remembers its last position. If you open the Offset page to modify Tool 3, don't just start typing numbers. Look closely at the screen to ensure your highlight bar is actually resting on Row 03. It is incredibly common for a tired operator to accidentally modify Tool 1 or Tool 2 because they forgot to use the directional arrow keys to move the cursor down first.Confusion about INPUT and INSERT keys?
INPUT and INSERT keys look very similar, but they perform completely different actions and target two entirely different areas of the machine's memory. The easiest way to understand the difference is to look at where your cursor is sitting on the screen: INSERT is for writing text files (Programs), while INPUT is for modifying settings (Offset tables and Parameters).INSERT KEY:
The INSERT key is exclusively used when your screen is displaying raw text lines of G-code either while writing a permanent program in EDIT mode or typing a temporary line in MDI mode.INSERT takes whatever is sitting in your bottom text typing buffer and drops it right after your flashing yellow cursor. It safely squeezes the new text into the program without erasing any code that comes after it.
When to use it?
1. Creating a new program head (e.g., typing O0112 and pressing INSERT).2. Adding a new block of movement commands (e.g., typing G01 X100.0 F500 ; and pressing INSERT).
3. Adding notes or comments inside brackets.
If you are looking at lines of text with G and M codes, always use INSERT to add your code. If you use INPUT on a program page, most modern machines will throw an error or do nothing at all.
INPUT KEY:
The INPUT key is used when you are navigating data matrix grids, such as your Tool Geometry (Length) table, Wear table, G54–G59 Work Offsets, or system Parameters.INPUT does not slide text around. It acts like a destructive wipe. Whatever number was previously saved in that highlighted cursor box is instantly thrown in the trash, and your new number takes its place entirely.
When to use it?
1. Setting your G54 X or Y coordinates manually (e.g., typing -400.500 and pressing INPUT).2. Typing a raw tool length measurement directly into your Geometry table.
3. Adjusting system variables or settings.
If you are looking at a grid table full of decimal numbers (Offsets), always use INPUT to save your numbers. (Pressing INSERT here will not register the data into the machine's calculation matrix).
0 Comments