Brandon Fowler

What does a G81 code do?

G81 calls a standard drilling canned cycle. 

It is a modal function that allows the machine (lathe or mill) to perform a one-pass drilling operation and retraction.

The machine will drill the hole in one straight shot and then retract out of the hole. There is no dwell or movement of the cutter away from the surface of the hole.

Just like other modal functions, you will need to deactivate it by calling another G code of the same type (canned cycle) or by using the G80 canned cycle cancel command to stop drilling.

When to use a G81 code?

The G81 command is useful when you want to drill holes that are not too deep and can be drilled in just one step.

G81 is the most common drilling canned cycle used.

G81 can be used for spot drilling, counterboring, reaming, boring, center drilling and other drilling operations. It is a very simple drilling cycle.

The G81 canned cycle does not include any retract steps (pecks) when drilling.

For this reason, if you want to drill a deep hole, the best option would be to use the G83 peck drilling deep hole canned cycle.

Peck drilling will help clear chips.

Other codes used with the G81 code

• G98 – Return to initial plane
• G99 – Return to R plane
• X – Hole location in X-Axis
• Y – Hole location in Y-Axis
• Z – Z axis location of the bottom of drilling motion
• R – Position of the retract plane (for movement clearance)
• F – Feed rate for drilling

G81 code format

The format for using a G81 command is shown below:

G98 (or G99) G81 X2.0 Y3.0 R1.0 Z-5.0 F25.0

It would be easy to assume that the Z location is the location of the start of the hole. In reality, it is the Z location for the bottom of the hole drilling movement.

Keep in mind that the X and Y coordinates of the hole are not usually in the same line as the G81 command.

In most programs you will see the G81 code in this format:

X2.0 Y3.0

G98 G81 R1.0 Z-5.0 F25.0

The program first identifies the coordinates of the hole and then starts the drilling process.

What to think about when using a G81 code?

Retract planes

The retract plane is the location that the machine will return to after each canned cycle.

There are two codes that affect retract planes. 

The G98 code will cause the machine to return to the Z location at the start of the canned cycle. The G99 code will tell it to return to the R plane.

Selecting a retract plane that is above any potential obstacles in the machine such as fixtures, clamps, or the part itself will allow the machine to safely move between each hole drilling location.

If the R plane is too low it could cause damage on the workpiece and lead to disaster. However, if an R plane is too high above the workpiece’s surface, it could increase machining time, due to the extra time needed to go all the way up to the R value after each drilling. 

Positioning mode

When using the G81 drilling cycle, you will need to be aware of the positioning mode that is currently active.

If G90 is active, the machine will read all locations as relative to a single zero location.

If G91 is active, the machine will read all locations as relative to its current position.

Pay careful attention to your current positioning mode because using the wrong one can easily result in a machine crash.

How to cancel a G81 code?

The G80 command is used to cancel a G81 code as well as all other canned cycles.

If the G81 command is not canceled, then the machine will continue to drill holes in every location given in the program.

G81 vs similar canned cycles

The G81 command is the simplest drilling canned cycle.

Besides G81 there are a few other G-codes for drilling holes with slight variations in the drilling process which make them better to use in certain circumstances.

Want to learn more about CNC G Code?

What does a G74 code do?

A G74 command activates the reverse, or left-handed tapping canned cycle.

Tapping is threading the female portion of a mating pair. Basically, this means you are creating the thing that will be screwed into.

Tapping is done by rotating the spindle, which holds the tap, down through the hole until it reaches the desired depth (bottom of the hole). 

When reverse tapping, the spindle should always be set to the counterclockwise direction with the M04 command.

Once at the bottom of the hole, the spindle will change directions and reverse out of the hole.

The G74 code is also used for peck tapping. Peck tapping is similar to peck drilling where the machine will tap in steps.

For instance, if your peck depth was 0.1” then the machine would feed down 0.1” and then back up. Then the machine would feed down to 0.2” and back up. Rinse and repeat going 0.1” lower with each peck.

Other codes used with the G74 code

When using a G74 code you need to consider all the aspects that control the tapping process, these are:

• G98 – Return to initial plane
• G99 – Return to R plane
• X – Hole location in X-Axis
• Y –  Hole location in Y-Axis
• R – The distance from the initial level to point retract (R) plane
• Z –  Final tapping depth
• Q –  Depth of cut for each peck
• F –  Cutting feedrate, this will be the pitch of your thread
• K (or L): The number of repetitions of the cycle

The retracting value (R) or clearance level refers to the plane perpendicular to the Z-axis where the tool can move safely from one hole to another. 

The R value should be set so the machine will clear any and all obstacles including clamps, fixtures and the part itself.

G74 code programming format

The format for using a G74 command is shown below:

G98 (or G99) G74 X2.0 Y3.0 R1.0 Z-5.0 F25.0

It would be easy to assume that the Z location is the location of the start of the hole. In reality, it is the Z location for the bottom of the hole tapping movement.

Keep in mind that the X and Y coordinates of the hole are not usually in the same line as the G74 command.

In most programs you will see them in this format:

X2.0 Y3.0

G98 G74 R1.0 Z-5.0 F25.0

The program first identifies the coordinates of the hole and then starts the tapping process.

How to cancel a G74 code?

The G74 code is canceled with the G80 command.  

If the G74 code is not canceled, the machine will try to tap a hole at every new location given in the program.

When to use a G74 code?

The G74 code is used when you want to tap an existing hole in a part.

Never use the G74 command to drill a hole. 

This operation is only meant to remove the material that will form the threads of the holes, not create the hole as well.

What to think when using a G74 code?

Speeds and feeds

You will need to set the spindle speed before using the G74 cycle. When using G74, the spindle should always be moving counterclockwise through the use of an M04 command.

The feed rate of code G74 will be the pitch of your thread.

Various holds or overrides for speeds and feeds will not work when tapping. This is for safety purposes.

Hole size and location

Before using the G74 there must be a previous drilling cycle.

The correct hole diameter for a tapping operation will be the final diameter of the screw minus the pitch. For example, the diameter of the hole for an M10 x 1.5 mm hole will be 8.5 mm.

Keep in mind that the X and Y coordinates of the hole are not usually in the same line as the G74 command. The standard format for selecting your hole location and calling the G74 tapping cycle is shown below:

X50.0 Y50.0

G74 Z-40.0 R5.0 F20

The machine is moved to the location of the hole to be threaded and then the hole cycle is used.

Retract planes

The G74 command is usually followed by the G98 code in the same line of code, in which case the machine will use the Z coordinate (height of the first hole) to move between holes.

When tapping it is advisable to set your R plane higher than usual.

CNC machines are capable of switching between modes very quickly, but the change is not instantaneous. 

The higher R plane gives the machine time to stabilize and ensure it is working at the correct feedrate before starting the cut.

G74 Rigid tapping

Rigid tapping means that the tap can remain rigid throughout the cycle. The machine spindle locks in with the feedrate similar to the screw cutting process.

There are tapping heads specially designed for this process.

To perform Rigid Tapping, the machine should be able to synchronize feed motion and spindle speed. This option may not be available on all machines, especially older ones. Check your machine manual to make sure you are capable of rigid tapping.

However, Rigid Tapping mode can cause issues due to chips sticking to the tool or increased cutting resistance. That’s why it is important to consider peck tapping.

G74 Peck Tapping

Including the Q parameter in the G74 command line will immediately set the machine to a peck tapping cycle.

This means that the spindle will rotate to a specified depth (Q value) in each tapping peck and then repeat the process, one step or “peck” at a time until reaching the bottom of the hole.

Peck tapping allows chips to exit the hole, making the tapping process easier and safer. 

The downfall of peck tapping is that it increases machining time when compared to standard tapping.  

G84 vs G74

The G74 cycle is the left-hand tapping cycle, sometimes called the reverse tapping cycle.

It performs the same operation as the G84 command but with the difference that the spindle rotates counterclockwise instead of clockwise.

The G74 left hand tapping cycle creates left hand internal threads while the G84 canned cycle creates standard or right-hand internal threads. Left hand threads are the opposite of your standard threads.

If G84 creates threads that are lefty-loosey, righty tighty then G74 creates threads that are righty-loosey, lefty tighty. In other words, G74 creates threads that would be screwed in the opposite way of normal.

The G74 command also has the ability to peck tap.

Both the G74 and G84 commands are modal commands which means they will stay on and in effect until they are either changed or canceled.

The cancel code to use with both cycles is G80.

G74 code example

G00 X50.0 Y50.0

G74 Z-40.0 R5.0 F20

X25.0

Y25.0

G80 Z10.0

M30

In this example, the tool approaches the coordinates of the first hole (X50 Y50), then starts the tapping process.

The tapping operation is set to reach a depth of 40 mm and has a retraction plane of 5 mm above the workpiece. This procedure is repeated in 2 more holes in the positions (X25, Y50) and (X25, Y25).

The program stops the tapping cycle by using the G80 command.

Finally, the tool moves away from the part in the Z axis and the M30 command ends the program.

Want to learn more about CNC G Code?

What does a G73 code do?

G73 is a modal command that sets the CNC machine to run a peck drilling cycle.

The practice of peck drilling refers to drilling a hole in a series of steps (pecks) instead of drilling the complete depth of the hole in a single pass.

G73 tells the CNC to retract a small amount after each peck. This helps break chips.

Difference between peck drilling and standard drilling

The main difference between peck and standard drilling is that the peck drilling process removes the material in multiple steps, while standard drilling is a one-step process.

Both commands are intended to make holes, but the peck drilling cycle allows more control over how the hole is drilled.

Peck drilling is the first option for CNC programmers when making blind holes. 

The pecking process helps break chips as well as remove them and any other debris from the hole during the drilling process.

Trouble removing chips from the hole when drilling can cause size and/or surface finish issues.

Standard drilling is far more common when dealing with simple through (thru) holes.

Parameters used with a G73 code

• F – Feedrate
• R – Position of the R plane (clearance level)
• X – Hole position in X-Axis
• Y – Hole position in Y-Axis
• Z – Position of the Z Axis at the bottom of hole
• Q – Depth to increase on each depth
• K or L – Number of cycle repetitions

The feed rate (F) is dependent on the material that is being cut and the diameter of the drilling tool that you are using.

The retracting value (R) or clearance level refers to the plane perpendicular to the Z-axis where the tool can move safely from one hole to another.

Also, some machines might use L instead of K for cycle repetition (depending on the model and machine type). If you are the programmer, remember to check the machine’s manual for further details.

An example G73 code would look something like:

G73 X2 Y3 R1 Z-5.0 Q1.0 F25.0 L2

How to cancel a G73 code?

The G80 command is used to cancel a G73 code as well as all other canned cycles.

If the G73 command is not canceled, then the machine will continue to drill holes in every location given in the program.

Is the G73 code the same on a lathe as a mill?

No, the G73 code performs a different function on a CNC lathe.

On a lathe, the G73 code is used for a pattern repeating cycle. The machine will cut the same pattern multiple times, stepping in on each pass.

When to use G73 code?

If you want to make a shallow hole, you won’t probably need the G73 code.

There is no need for the tool to take on several pecks if the depth of the hole is less than an inch (depending on the material and tool).

The G73 command works best when you follow a general rule: 

If the depth of the hole is 3 to 4 times greater than its diameter, use a peck drilling cycle such as G73.

G73 vs G83

The most similar code to G73 is G83.

Both are peck drilling cycles with one key difference.

G83 will retract completely out of the hole after each peck to the retract plane. G73 will only retract to the start of each peck.

The G73 canned cycle is a peck drilling cycle but with a shorter retract intended for relatively shallow holes. Meanwhile, the G83 command is peck drilling with a full retract intended for deep holes.

Both commands are meant to help break and clear chips. G83 does a better job of this by fully retracting out of the hole but with the added expense of a longer cycle time.

On the other hand, G73 is designed to break up stringy chips, while G83 is intended to pull chips up and out of deep holes.

G73 vs similar codes

Besides G83 there are a few other G-codes for drilling holes with slight variations in the drilling process which make them better to use in certain circumstances.

Want to learn more about CNC G Code?

What does a G43 code do?

The G43 code turns on tool length compensation.

Tool length compensation allows the CNC machine to account for the length of your cutting tool that has been entered and stored in an H offset value.

H offsets and G43

The G43 command tells the machine to turn on tool length compensation, but it is the H code that tell the machine how much to compensate for.

The H offset number will correspond to a value stored in the machine’s memory, often entered at the time of setup. This value will be for the length of the tool. The memory storage location is often called an offset table or library.

There are multiple H offsets that can be stored in the tool table. Each tool will have its corresponding H offset value.

The best practice when storing offsets is to match the tool number with the H number. This means for tool #1 you will store the tool length offset in H01. For tool #2 you will store the offset in H02 and so on.

How to use a G43 code

You know the G43 code is used in a CNC program to account for the tool length, but why does it matter?

It matters because without a G43 code, you would need to create a new program every time you wanted to run the same part with a different tool.

An H code is used with the G43 code to select the height (H) offset value. The H code tells the CNC which H (height) offset value to account for when running the program.

This allows any number of tools to be used in the same program as long as your controller stores enough offset values and those offset values have been entered correctly.

When a G43 code is not active, the machine will move the end of the spindle to all locations in the program.

When the G43 code is active, the machine will move the end of the cutting tool to all locations in the program.

You can see how not having the G43 code on when needed could cause a crash. You are trying to move the end of the spindle to a new location and if a tool is loaded in the spindle then it is in the way of that movement.

This can mean you end up with a damaged part, broken tool or maybe even damage to your CNC.

Where does the G43 code show up?

G43 will often be used at the start of a new section of code.

This will ensure that you have tool length compensation on and the correct H offset applied before running that section of code.

Making sure they are on and set to the correct offset will allow you to run only that section of code if needed.

This can be helpful if a particular feature or size of the part being worked doesn’t come out as intended. It is common to need to rerun only a section of your CNC program to dial in the size.

To make sure this is possible you need to make sure your machine is always set to the correct modes using modal commands.

G43 is one of those modal commands, which means it stays active until switched or canceled. The same goes for many other g codes.

The best practice when dealing with modal commands is to not assume that they will be on when you need them. 

You should call them out in any section of your program where they will be needed. This practice is called using safety lines or safety codes in your program.

It is better to be safe and include them than to not and be sorry when your machine crashes.

How to format your G43 codes

There are three parts to your G43 code.

The G43 code itself, the H offset number to use, and a location move.

Altogether they should look similar to this line of code:

G43 H02 Z1.0

In this example G43 turns the tool length compensation on using the 2^nd H offset value and moves the machine to a location 1 unit above the Z axis zero location.

Note that tool length compensation with the H02 offset for all future moves until it is turned off or changed.

How to cancel a G43 command

G49 is the command that cancels tool length compensation.

It will cancel any active G43 or G44 modes that may be active.

G49 is often used at the beginning of the program as part of the safety lines or safety block of code that initializes the machine and makes sure all of the correct modes are set.

What to think about when using a G43 code

When using a G43 code the most important thing to think about is avoiding collisions.

Correctly using the G43 code will also help make sure that your parts come out the right size.

The G43 code will take effect on your first Z axis move after using the G43 code. This will usually all be the same line of code.

You want to avoid getting too close to your part before calling out the G43 code. Call out your tool length compensation while you are still a safe distance away from your workpiece to avoid crashing your machine.

G43 vs G44

G43 and G44 are opposites.

One is a positive compensation, and the other is a negative compensation.

G43 tells the control to adjust for a positive length compensation.

G44, which is rarely used by most shops, tells the control to adjust for a negative tool length. 

I wouldn’t worry about understanding why or how to use G44 if you are just starting out. Get a little experience under your belt before worrying about this rarely used code.

CNC codes that are similar to G43

We established that G44 works much like a G43 code but what other similar codes are there available.

The other main types of cutter compensation are the G41 – Cutter Compensation Right and G42 – Cutter Compensation Left. 

These cutter compensation codes allow the machine to account for the diameter of the cutting tool. Which one gets used depends on the type of cutting you are doing.

Climb milling will use the G41 code. Conventional milling will use the G42 code.

The cutter compensation G codes G41 and G42 adjust for the diameter of the cutter while G43 accounts for the length of the tool.

Please note that G41 and G42 are also modal commands, which means they will stay on until turned off or switched.

G43 code example

Check out the G43 code example below to see how the code affects what the machine will do.

The N numbers below, such as N100, are line numbers for your program. Some programs might not include them, but we left them in so they don’t confuse anyone.

Example #1:

N100 T02 M6                                   

N105 G00 G43 H02 Z1.0

N110 G01 Z-2.0 F5

Line 100 selects tool #2 and changes to that tool.

Line 105 sets the movement mode as rapid and turns on tool length compensation while moving to Z = 1.0

Line 110 sets the movement mode as straight line movement and moves the tool to Z=-2.0 at a feed rate of 5 units per minute.

Want to learn more about G Code for your CNC?

What does a G42 code do?

G42 is a modal command called cutter compensation right.

This code adjusts the path of the cutting tool based on the diameter of the cutter.

If you are looking towards the direction that the cutter is moving, the tool path is shifted to the right.

There are also codes for using no cutter compensation (G40) as well as using cutter compensation left (G41).

What is cutter compensation?

Cutter compensation is a CNC mode that allows the CNC controller to adjust for the size of the cutting tool.

Setting the size of the cutting tool allows you to use the same program with multiple different cutting tools.

Turning cutter compensation on tells the machine to shift the cutting tool either left with G41 or right with G42. The shift is half of the diameter of cutting tool, otherwise known as the radius.

Visualizing which way the machine will shift can be a little tricky. The shift happens as if you are looking towards the direction that the cutter is moving.

G41 vs G42

There are two different cutter compensation modes that can be used:

• G41 for cutter compensation left
• G42 for cutter compensation right

The direction of the shift is relative to the cutting tools direction of movement.

G41 is used when climb milling, which is the most common type of milling used.

G42 is used when conventional milling. Conventional milling sounds like it would be the standard but in reality, it is rarely used.

When climb milling, the cutter moves in the same direction as the stock feeds, which means that the workpiece produces less resistance to the cutting as the chips fall behind the cutter.

This type of milling helps prolong the life of the cutters and creates a better surface finish. This is the most commonly used milling method CNC machines.

On the other hand, with conventional milling the cutter runs in the opposite direction of the stock feed, which means that the cutter will have more resistance against the workpiece and cause more tool wear resulting in a shorter tool life.

The two images below show how the CNC will move when the other cutter compensation modes are active.

Advantage of using cutter compensation

The advantage of cutter compensation is that you won’t need to rewrite your program continuously to adjust for the size of your tool.

Imagine you bought a new end mill, and it came in 0.001” smaller than the last one. This would mean that your parts would now come out larger than before. To account for this you can use cutter compensation and your D offsets to tell the machine how big the cutter is.

This allows you to continue using the same program even though your cutter has changed.

Cutter sizes and D offsets

Even if you were to buy two of the same cutters, it is likely that there is a small difference in size between them. This difference in size is accounted for using offsets.

There are H offsets and D offsets that can be used when CNC machining.

Because we are talking about cutter compensation with G42, we are going to focus on D offsets.

D offsets are stored in your machine’s controller, and they store the diameter of your cutting tool.

Now usually when the machine reads the coordinates given in the program, it moves the center of the cutting tool to that position. This can make it difficult to get the correct size especially when using different or multiple cutters.

Telling the machine the size of the cutters with your D offsets allows it to account for them and run the same program with different tools and get the same size part.

If you didn’t have cutter compensation, then you would need to create a new version of the program every time you wanted to use a new tool.

Using Tool Offset Table for Cutter compensation

The Tool Offset Table, sometimes called Tool Table or Offset Library, is simply a table that the operator uses to store the offset values. This can include both diameter (D) and tool length (H) offsets.

Tool offset tables vary and some machines will only store one type of offset.

This means you may need to store both your diameter and tool length offsets in a D offset.

Some other machines may allow you to store the diameter and length of a cutting tool in the same offset number. The setup varies by machine so check yours out to make sure you know how it works.

The purpose of the Tool Table is to tell the CNC machine what the dimensions of the cutting tool are. This includes radius and length.

How to turn off cutter compensation

Cutter compensation with G42 is canceled by using the G40 code which cancels all active cutter compensation modes.

Alternatively, G42 can be canceled by switching to cutter compensation right by using the G41 code.

The two main things to pay attention to when using G40 to cancel cutter compensation are:

• Cancel cutter comp when you are off the part more than half the diameter of the cutter
• Make a move when canceling cutter compensation

Canceling off the part enough keeps the machine from running back into the part.

Making a move forces the machine to move in a consistent way. Some machines can react unexpectedly if no move is made when canceling cutter compensation. The machine basically thinks it has teleported location.

Don’t teleport your CNC. Make a move when canceling cutter compensation.

G42 programming format

There are multiple ways of formatting a G42 command:

1. G42 D1. When the G42 code is used with a D offset it is meant to be used on a machine with a built-in tool table in the controller. G42 turns on cutter compensation left and D1 tells the machine to adjust the tool path based on the size stored in the first D offset.
2. G42 P2. The P value is the radius of the tool used in the operation. This format is used more often on hobby level machines.
3. G42 X2. This format is the same as using the P value.

Focus on learning the first format unless you plan to only ever use simple home level machines.

Other types of compensation

The other main form of compensation is tool length compensation.

Tool length compensation is turned on with either G43 or G44. Although G44 is almost never used. G43 is by a super wide margin the most often used tool length compensation.

Tool length compensation accounts for the length of the cutting tool relative to the end of the spindle.

Tool length compensation is canceled with the G49 code.

Want to learn more about CNC G Code?