Learn Links in PowerMill Explained Simply – Safe, Incremental, Skim, On Surface, Stepdown, Straight and Circular Arc Moves

Introduction:

Every CNC programmer knows that the cutting pass is where the material is removed. That is the obvious part. But what happens between those cutting passes is far less obvious and surprisingly it is often where the most time is wasted and the most damage is done. While we obsess over feed rates, stepovers and toolpath strategies the humble connecting movement, the travel that occurs between cuts is frequently overlooked treated as an afterthought to be managed by default settings. This connecting movement is governed in PowerMill by a critical yet often misunderstood parameter: Links. A link is precisely what its name implies, the path the tool takes to move from the end of one cut to the start of the next. On the surface, it seems simple. In practice it is a complex balancing act between speed, safety and surface integrity.

PowerMill categorizes these links into two fundamental types, each with its own logic and risks. Short Links handle the rapid, local transitions between adjacent passes, the small hops that keep the tool engaged within a localized region. Long Links, on the other hand, manage the sweeping traverses across the entire model, moving the tool from one isolated pocket or feature to the next. Each type demands its own strategy.

The true art of configuring links lies in managing three competing priorities. First, there is cycle time, every unnecessary retract, every prolonged clearance move, adds seconds that compound into minutes and hours of wasted production. Second, there is surface quality, a poorly configured link that drags the tool across a finished surface will leave permanent, unsightly witness marks, ruining an otherwise flawless finish. Third and most critical is safety, a link set too low will crash the tool into a clamp or a steep wall while a link set too high will waste precious machining time.

Furthermore, the choice between a Rapid (G00) link and a Feed (G01) link is not merely a technical checkbox, it is a strategic decision. Rapids are fast but offer no collision detection if something goes wrong. Feed moves are slower but far more predictable and can be carefully traced along safe, verified paths. Knowing when to prioritize speed over safety and vice versa is the hallmark of an experienced PowerMill programmer.

Links:

In Autodesk PowerMill, Links control how the tool moves between separate cutting passes within a toolpath. While Leads handle how the tool enters and exits the material for a single cut, Links determine the connection moves when the tool lifts, repositions, or transitions to the next pass. Properly configuring links is crucial for reducing cycle time, preventing tool damage, and ensuring a good surface finish. To choose the right link, you have to balance two goals: preventing the tool from crashing (safety) and stopping the tool from wasting time cutting air (efficiency).

In PowerMill’s Toolpath Connections dialog, you will see options for First Choice, Second Choice, Apply Constraints, and Default.
PowerMill gives you these options because a single toolpath often contains many different types of gaps. These settings act as a decision tree (a logic flow) that tells PowerMill exactly how to handle different situations automatically.

1. First Choice vs. Second Choice:

This is your primary backup system. PowerMill looks at the distance between two cutting passes and decides which link option to use based on your preferences.

First Choice:

This is the link type you prefer to use because it is the most efficient.
e.g. You set First Choice to Stepdown or On Surface. PowerMill will try its best to use this link to keep the tool down and save time.

Second Choice:

This is your backup plan. If PowerMill calculates the First Choice link and realizes it is impossible or unsafe. For example, a massive wall is blocking the tool, or the next pass is too far away, it will fail the First Choice and automatically switch to your Second Choice.
e.g. You set Second Choice to Skim or Incremental. If the tool can't stay down on the surface, it will lift slightly and fly across.

2. Apply Constraints:

The Apply Constraints checkbox is the trigger that activates your First and Second choice logic. It allows you to set rules based on the distance of the gap.

• When you check "Apply Constraints," you can define a maximum distance (e.g., 10mm).

• If the gap is shorter than 10mm: PowerMill applies your First Choice link.

• If the gap is longer than 10mm: PowerMill skips the first choice completely and uses your Second Choice link.

e.g. 

Imagine you are finishing a part with small pockets.

• First Choice: Circular Arc

• Second Choice: Skim

• Constraint: Limit = 5mm.

If the tool finishes a pass and the next pass is only 2mm away, PowerMill says, "This is under 5mm, so I will make a smooth Circular Arc U-turn on the surface." If the tool finishes a pass and needs to jump all the way to a different pocket 50mm away, PowerMill says, "This is way over 5mm. A circular arc would be massive and dangerous. I will switch to the Second Choice and Skim through the air instead."

3. Default (The Ultimate Safety Net);

The Default link is the absolute baseline safety setting. It is the option PowerMill falls back on if both your First Choice and Second Choice fail or are deemed unsafe by the software's automatic gouge-checking algorithm. By default, PowerMill usually sets this to Safe.

If you tell PowerMill to try an On Surface link (First Choice), but an unexpected fixture clamp is in the way, the software realizes it will crash. It then looks at your Second Choice (Skim), but realizes the tool will still clip the clamp. PowerMill says, "Both user options are dangerous. I am overriding them and using the Default (Safe) link to lift the tool entirely into the sky."

To visualize how these Links work intuitively, imagine the tool is a hiker walking along mountain ridges (the cutting passes). The hiker needs to get from the end of one path to the start of a new path.

Here is how each link option behaves in that scenario:

1. Safe:

The Safe link option forces the tool to retract all the way up to the defined Safe Area or Safe Z plane before moving rapidly to the start of the next cutting pass. Use this when there are large, complex obstacles, clamps, or unmachined material between the two passes. It is the most conservative and secure option, but it adds the most non-cutting air time.

Tool cuts → Retracts vertically to Safe Z → Moves rapidly (G0) horizontally → Plunges vertically to the start of the next pass.

Imagine the hiker finishes a path, calls a helicopter to lift them completely up into the clouds (Safe Z), flies horizontally over the entire mountain range, and then drops straight down to the start of the next path. It is 100% safe because you are flying way above any peaks or trees, but it wastes a massive amount of time waiting for the helicopter to go up and down.

How High Does It Lift?

Safe lifts all the way to a fixed, absolute ceiling called Safe Z.Found under the Safe Area tab. It calculates a plane high enough to clear your entire raw block of material plus a safety margin (e.g., 10mm or 20mm above the highest point of the whole part).

When to use:

• When there is still a massive, unpredictable chunk of metal on the machine table.

• When you have physical clamps, fixtures, or high unmachined walls standing directly between your cutting passes.

• If you are leaving the machine to run overnight and cannot risk a crash.

2. Incremental:

An Incremental link retracts the tool to a specified distance above the local part surface rather than going all the way to the Safe Z plane. The tool retracts to a clearance height calculated relative to the surrounding geometry, moves horizontally, and plunges back down. Excellent for flat or relatively uniform areas. It saves significant cycle time compared to Safe because the tool doesn't travel all the way up into the air between passes.

Instead of a helicopter, the hiker puts on spring-loaded stilts that instantly lift them exactly 10 feet above whatever ground is directly beneath them. They walk at that fixed height above the terrain, then step back down. Much faster than a helicopter because you only lift as high as necessary to clear the local ground, but you still have to do a lot of stepping up and down.

How High Does It Lift?

Incremental lifts a user-defined distance above the local component surface.Found under the Moves and Clearances or Z Heights tab. If your clearance is set to 5mm, the tool lifts exactly 5mm above the surface at that specific spot before moving.

When to use:

• When you are pocketing or facing a part where the floor is relatively uniform.

• Open areas with minor steps, where the tool needs to hop over small steps or ribs but doesn't need to climb all the way out of the machine to do it.

3. Skim:

A Skim link is a highly efficient high-speed clearance move. The tool lifts slightly off the finished surface to the "Skim Distance", clears any remaining stock in a high-speed linear move, and drops back into the next pass. PowerMill uses the 3D model to calculate a safe, low-flying boundary. It is ideal for high-speed machining (HSM). It minimizes air cutting and keeps the machine tool moving fast, but relies heavily on accurate stock models to avoid collisions.

Here our hiker transforms into a low-flying drone. They lift just a tiny bit off the ground say, 1 inch and zoom at maximum speed, effortlessly contouring just above the mountain peaks to get to the next spot. This is the ultimate time-saver for roughing. It keeps the tool as low to the part as safely possible and moves at maximum machine speed (G0 or high feed) without wasting time climbing into the sky.

How High Does It Lift?

Skim lifts just a tiny bit to clear the model, relying on a 3D boundary map.You set a Skim Distance typically 2mm to 5mm. PowerMill looks at the 3D shape between Point A and Point B, finds the highest obstacle on that specific line, and flies exactly the Skim Distance over that peak.

Skim is smart. Instead of lifting to a fixed plane, it acts like a drone scanning the terrain. It lifts just enough to "skim" over any obstacle directly in its line of sight, doing the horizontal travel at maximum rapid machine speed (G0).

When to use:

• This is the industry-standard choice for modern high-speed roughing (like PowerMill's Vortex strategy).

• Deep Cavity/Pocket Clearing, where the tool finishes a pass inside a pocket and needs to rapidly move to the other side of the pocket without lifting all the way out into the air. Your machine must be capable of fast rapid movements (G0 or high G1 feed rates).

4. On Surface:

The On Surface link keeps the tool in contact with or microscopic distances away from the component profile between passes. Instead of lifting into the air, the tool follows the contour of the part geometry to get to the next starting point. It is used in 3D finishing operations like Scallop or Constant Z on smooth, continuous surfaces. It eliminates witness marks caused by the tool constantly retracting and plunging back into the material.

Our hiker never leaves the ground. When one path ends, they simply walk along the face of the mountain, hugging its curves, until they reach the next path. Since the tool never lifts off the metal, the machine doesn't vibrate from constantly retracting. This prevents the tool from leaving ugly witness marks or small gouges on a beautifully finished mold.

When to use:

• Mostly used in 3D Semi-Finishing and Finishing, crucial for strategies like Scallop, Constant Z, or Isometric projection finishing on complex molds, dies, or organic shapes like car body panels.

• When surface finish is critical, where every time a tool lifts off a finished metal surface and plunges back in, it leaves a tiny visible mark (a witness mark). "On Surface" keeps the tool down, gliding smoothly onto the next pass to eliminate those marks.

How High Does It Lift?

On Surface acts like a rollercoaster hugging a bumpy surface. it keeps tool in contact or lifts small distance away from material througout it's movement. It just follow surface, if it encounter a flat surface it will move along it and if it encounter a bumpy surface ahead it will move along it.

An On Surface link does not lift up into the open air, but it also does not aggressively rub or cut the part under heavy pressure. Think of it as the tool lightly skimming or tracing the exact shape of the finished part as it moves to the next pass.

Here is exactly how it behaves mechanically:

1. It stays locked to the part geometry. Instead of retracting vertically into the sky, the toolpath calculation forces the tool to follow the 3D contour of your model. If there is a curve, a slope, or a flat floor between Pass A and Pass B, the tool will glide along that exact contour.

2. Does it actually touch the metal?
Technically, it is right at the finished surface boundary (Z=0 stock remaining). Because the tool spindle is spinning, it might lightly graze or dust the surface as it moves, but it is not taking a heavy depth of cut. To give programmers absolute control and protect the part, PowerMill includes a hidden safety feature inside the On Surface settings called Gouge Check and Clearance.

3. Most experienced programmers don't let the tool literally scrape the finished metal while linking because a tiny bit of machine vibration could leave a faint scratch. Instead, inside PowerMill's Link settings, you can look for the option to add a tiny clearance to your On Surface links often handled automatically by the software's gouge-protection algorithm. This keeps the tool 0.05mm to 0.1mm in the air right above the surface.

4. It is aligned to the part. It follows the exact 3D shape of the model, riding just a microscopic fraction of a millimeter above the finished metal or kissing the surface so it can transition to the next cut without leaving a plunge mark.

5. Stepdown:

A Stepdown link is specific to situations where the tool needs to transition to a lower Z-level common in waterline or Constant Z machining. Instead of lifting up and plunging back down at the new depth, the tool moves directly down the wall or profile from the end of one level to the start of the next. It is used in roughing or Z-level finishing to keep the tool down in the cavity or around the core, minimizing vertical Z axis movement.

Imagine you are machining a pyramid from the top down, circling around it. When you finish the top loop, instead of lifting up into the air to start the second loop, you simply step down the side of the wall to the next level. It treats the vertical depth change like a natural continuation of the cut, keeping the tool down in the action.

To understand Stepdown, you have to think about Z-Level Machining. This is where the tool cuts in horizontal slices, moving from the top of the part down to the bottom like slicing a loaf of bread horizontally.

Imagine you are machining a hollow bowl or a pocket:
1. The tool finishes cutting a complete circle at the very top level (Depth: -5mm).
2. Now, it needs to move down to start the next circle (Depth: -10mm).

Without Stepdown (Using "Safe" or "Skim"):

The tool finishes the -5mm circle → Lifts all the way up into the air → Moves over → Plunges down to -10mm → Starts cutting.
This wasting a lot of time moving up and down in the air.

With Stepdown:

Instead of lifting into the air, the tool stays down against the wall of the bowl. It simply feeds straight down or slides down at an angle along the surface from -5mm to -10mm and immediately starts the next cut.

In short, stepdown is a link used specifically when moving downward to the next cutting depth. It tells the tool: "Don't lift up into the air; just step down to the next level right here against the material."

How High Does It Lift?

Stepdown perform no lifting up, instead of lifting up into the air, Stepdown is used when the toolpath is a sequence of downward stairs. The tool cuts a loop, and then simply slides down the vertical wall of the material to start the next lower loop. It is exactly equal to your Stepdown (axial depth of cut) setting for that toolpath strategy (e.g., if you are cutting down 2mm at a time, it steps down 2mm).

When to use:

• Mostly used in Waterline / Constant Z Machining, where your toolpath cuts a single horizontal loop around a core or inside a cavity, and then needs to move immediately to the next loop directly underneath it.

• When slicing down a vertical wall in steps, keeping the tool down in the cut rather than retracting between depth levels.

6. Straight:

A Straight link connects the end of one pass to the start of the next with a direct, straight line in 3D space. The tool moves linearly from point A to point B without any arcs or surface-following geometry. it is typically used when the distance between passes is very short and there is absolutely no material or obstacle in between. If used carelessly over a feature, the tool will cut straight through it.

The hiker builds up a zip-line directly from the end of Path A to the start of Path B and goes in a perfectly straight line. It is the shortest possible distance. However, if there is a mountain peak standing between Path A and Path B, the zip-line will crash straight through it. You only use this when you are 100% sure the path between the two points is wide open.

How High Does It Lift?

Straight does not lift at all. There is no height setting because it doesn't lift. It draws a perfectly straight line through 3D space directly from the end of the last cut to the start of the next one.

When to use:

• Used in very short gaps where the distance between the end of pass A and the start of pass B is incredibly small (e.g. less than 1–2 mm).

• Only use this when you are absolutely sure there is a wide open gap or slot between the two paths where no material exists.

• Never use this as a global setting; use it only as a Short Link choice for tiny transitions.

7. Circular Arc:

A Circular Arc link connects two passes using a smooth, tangential radius. Instead of sharp, angular turns or straight lines, the tool blends out of one pass and into the next using a circular arc trajectory. It is essential for high-speed machining. Sharp direction changes cause the CNC machine to decelerate, increasing cycle time and leaving tool marks. Circular arcs maintain a constant feed rate, reduce machine vibration, and extend tool life. This protects the machine. By smoothing out the link into an arc, the CNC machine doesn't have to jerk or slow down. It maintains high speed, reduces wear and tear on the machine spindle, and prevents tool breakage.

Imagine a racecar finishing a lap. If it tries to make a sharp, 90-degree square turn to get to the next lane, it has to slam on the brakes, turn, and accelerate again. A Circular Arc replaces that sharp corner with a smooth, sweeping U-turn.

A Circular Arc link is all about smoothing out sharp corners between passes to keep the machine moving fast.
Imagine you are mowing a lawn. You reach the end of one straight row, and you need to start the next row right next to it. You have two choices:

1. The Sharp Way (Straight/Common Links): 

You stop completely, turn exactly 90 degrees, walk over one step, stop completely again, turn 90 degrees, and walk back. (This is jerky and slows you down).

2. The Smooth Way (Circular Arc): 

You walk to the end of the row and make a smooth, continuous U-turn (like a loop) to blend right into the next row without stopping.

By choosing Circular Arc, PowerMill adds a tiny, smooth radius curve between the end of Pass A and the start of Pass B. The machine can maintain its high speed smoothly through the turn without jerking.

How High Does It Lift?

You specify an Arc Radius in the settings. If you set a 5mm radius, PowerMill swings the tool out in a smooth 5mm curve to blend the end of one pass right into the start of the next.

When to use:

• When connecting parallel passes like a Raster or Z-Level finishing pass where the tool must make a U-turn to head back the other way.

• Use this on heavy or high-speed CNC machines to prevent the axes from shaking, jerking, or banging when changing directions. It keeps the machine movements fluid and quiet.

EXAMPLE:

Let's visualize how Links works during machining of pocket and how PowerMill paths actually transition that will make it click perfectly.

1. The Approach (Leads):

The tool starts outside the part. It approaches horizontally and uses a Horizontal Arc Lead-In to smoothly blend into the cut.

2. The Cutting Pass:

The tool cuts around the pocket, moving inwards toward the center.

3. Moving Back Outside (The Link):

Now the tool is at the center of the pocket at Layer 1 (say, Z=−5mm). It needs to get back outside the pocket to start Layer 2 (Z=−10mm).

• To cross over the pocket wall and get back outside, it MUST use a Link, since it is moving through non-cutting space.

• If you choose Safe: It lifts out of the pocket to the sky, flies outside, and drops down.

• If you choose Skim: It lifts a few millimeters, fast-travels over the wall of the pocket, and goes outside.

• If you choose On Surface: It stays down and literally rolls up and over the wall to get outside.

4. Going to the next depth (Stepdown vs. Plunge):

Here is the minor correction: Once the tool has traveled back outside the part, it is sitting in open air. To go down to the next layer (Z=−10mm), it doesn't need to plunge harshly. It uses a Stepdown Link or a vertical plunge before it begins its next Horizontal Arc Lead-In.

You separated the horizontal move back to the start from the vertical move down to the next layer.

1. In PowerMill, you actually tell the software exactly this by setting a First Choice Link and a Second Choice Link:

2. First Choice Link = Stepdown: If the start of Layer 2 happens to be right directly below where Layer 1 ended, PowerMill will just use a Stepdown link to slide straight down the wall.

3. Second Choice Link = Skim / Safe: If the tool has to travel all the way across the pocket to get back outside like in your example, the Stepdown link fails because it's too far. PowerMill automatically switches to your second choice (Skim or Safe) to lift the tool up, fly it back outside and then drop it down to the next depth.



To help you fully master these concepts, let’s look at a series of distinct machining examples. Each example represents a common real world problem where one specific link option is the clear winner.

1. Machining an Engine Block with High Clamps:

You are face-milling the flat top surface of an engine block. However, the part is held down tightly on the machine bed using two thick steel step-clamps that stick up 30mm higher than the top of the block. The toolpath needs to transition from cutting the left side of the block to the right side, meaning it must cross over the area where a clamp is bolted down.

You must use Safe. The tool finishes cutting the left side, retracts all the way up to the Safe Z plane (e.g., 50mm above the part), flies right over the top of the steel clamp in mid-air, and then plunges down on the right side to resume cutting.

Skim or Incremental would calculate height based on the engine block surface, totally ignoring the physical clamp height, resulting in a catastrophic crash into the steel fixture.

2. Cleat Holes in a Flat Plate:

You are pocketing out five individual bolt holes arranged in a line across a perfectly flat steel plate. Once Hole #1 is completely hollowed out, the tool needs to move 100mm up the line to start cutting Hole #2.

You use Incremental with a clearance height of 5mm. The tool finishes Hole #1, lifts up exactly 5mm above the flat face of the plate, rapids across the smooth steel surface, and drops into Hole #2.

It’s efficient, because the plate is perfectly flat, you already know there are no obstacles between the holes. Using "Safe" would make the machine waste hours climbing up and down into the sky for all five holes.

3. Deep Cavity Mold Roughing:

You are roughing out a complex plastic injection mold cavity using a high-speed strategy like Vortex. The toolpath looks like a massive maze of squiggly lines inside a deep pocket. The tool finishes a tiny corner on the left side of the cavity and needs to jump over to a corner on the right side. There are unmachined "islands" of stock left standing in the middle of the pocket.

You use Skim with a 2mm skim distance. The tool retracts just 2mm higher than the tallest remaining island of metal inside that pocket, flies across at maximum high-speed feed rate (G0), and immediately drops back into the next cut. It keeps the machine in its high-speed comfort zone. The tool stays deep inside the pocket cavity, never wasting time retracting up into the open air above the mold block.

4. A Smooth Car Hood / Bonnet (3D Finishing):

You are running a final Scallop finishing toolpath over a wide, organic, curved car hood panel. The surface finish needs to look like a mirror. The tool finishes one long, sweeping 3D curve and needs to step over 0.2mm to start the next parallel sweeping curve.

You use On Surface. Instead of lifting off the metal, the tool stays locked onto the metal, smoothly gliding sideways across the organic curve to start the next pass.

If you used Safe or Skim here, the tool would lift up and plunge down thousands of times. Every single plunge would leave a microscopic "dent" or mark on the car hood, ruining the cosmetic finish.

5. Cutting the Cooling Fins on a Cylinder Head:

You are machining deep, vertical slots like cooling fins on a motorcycle engine using a Constant Z or Waterline strategy. The tool cuts a complete loop around the outer profile of the fin. The loop at the current level is done. The tool needs to go down 1.5mm vertically to start the next lower loop.

You use Stepdown. The tool finishes Loop 1, stays flat against the vertical wall of the fin, and steps or ramps directly downward by 1.5mm to begin Loop 2.

There is absolutely no reason to pull the tool away from the part. Stepping down directly along the cut axis keeps the machine axes moving efficiently without any unnecessary air-cutting.

6. Parallel Raster Finishing on a Mold Core:

You are finishing a large, gently sloping core block using a Raster strategy i.e. moving back and forth like a lawnmower. The tool reaches the end of a straight line. It needs to step over a fraction of a millimeter and head back in the opposite direction.

You use Circular Arc. As the tool hits the edge of the pass, PowerMill creates a smooth, sweeping U-turn loop in mid-air to swing the tool smoothly into the returning lane.

It's critical because sharp change in direction causes a CNC machine to experience high acceleration forces, resulting in machine jerking and structural vibration. The circular arc allows the machine to maintain a fluid, continuous feed rate without slowing down or shaking.

7. Connecting Micro-Segments in Engraving:

You are engraving text onto a brass plaque. The toolpath is tracing the letter "H". It finishes the left vertical line and needs to move over a tiny fraction of a millimeter to start the center horizontal crossbar. The gap between the two lines is so minuscule that any lifting move is a complete waste of time.

You use Straight usually restricted as a "Short Link". The tool finishes the left line, cuts a perfectly direct, straight line through the air to the crossbar, and begins cutting immediately. For gaps under 1mm or 2mm where you are absolutely certain there is no material standing in the way, a straight line is the fastest possible bridge.

In Example 3 of The Offset Pocket, why you don't usually see links during those inward transitions between completion of outer rectangle and starting of inner rectangle while moving inwards, and what about spiral the tool will never lift till cutting complete,

How links is used there and how Spiral and Offset strategies change the game?

You are completely right about standard pocketing. When a tool cuts an outer rectangle and steps inward to the next smaller rectangle, it usually does not lift up or use an air link. Instead, PowerMill uses a Stepover. It finishes the outer ring and then diagonally or perpendicularly cuts through the material to start the next inner ring. Because the tool is constantly touching metal and cutting during this transition, PowerMill treats this as a Segment a cutting move, not a Link.

So when does Example 3 (Skim Link) actually happen?

The "Skim Link" situation happens when the geometry is not a perfect, simple rectangle.

1. Imagine a pocket that looks like a kidney bean, or a pocket with a giant island like a pillar standing right in the middle.

2. The tool clears out the left side of the pillar, stepping inward.

3. Suddenly, it realizes it cannot step inward anymore because the pillar is blocking the path. The remaining material is all the way on the right side of the pillar.
The tool is trapped. It cannot cut through the solid pillar to get to the other side.
This is exactly when it uses a Skim Link. The tool stops cutting, lifts up 2mm, flies at high speed over or around the pillar, drops back down on the right side, and resumes its inward offset stepping.

If the tool can reach the next pass by cutting its way there, it stays down (Stepover). If a wall or an island blocks its path, it must lift and use a Link like Skim to jump over the obstacle.

Spiral Cutting:

A true spiral is the holy grail of high-speed machining because the tool never stops cutting and never lifts up until the entire pocket is empty. In a continuous spiral toolpath, the toolpath is just one single, unbroken, continuous mathematical line that winds inward like a whirlpool. Because the line never breaks, there is no "End of Pass A" and "Start of Pass B." It is all just one long pass.

How are Links used in a Spiral?

In a perfect world with a perfect circular pocket, a spiral uses zero links during cutting. It only uses:

1. A Lead-In at the very beginning to enter the metal.
2. A Lead-Out at the very end at the center of the pocket to lift away.

However, links will reappear in a spiral path under two specific conditions:

1. If your shape is irregular. If you are spiraling inside a star-shaped pocket, the spiral will eventually break into separate segments when it reaches the tips of the star points. The tool will have to lift (Skim/Safe) to travel from one star point to another.
2. If there is an obstacle inside the pocket, the spiral is forced to split into two separate paths to go around it, requiring a link to tie them back together.

Then why not just plunge at the center where the tool finished Layer 1 and cut the second layer from the inside out?

1. While PowerMill can be forced to do this in certain strategies, CAM software defaults to moving back to the outside for one massive reason: Climb Milling vs. Conventional Milling.
To understand why this matters, let's look at how the tool rotates and cuts the metal.
Consider we set cutting direction to Climb Milling.

Outside-to-Inside: 

When a tool starts on the outside of a pocket and steps inward moving clockwise, it forces the machine to do Climb Milling. The tool teeth bite into the thickest part of the material first and spit the chips out behind them. This results in an excellent surface finish, low heat, and long tool life.

Inside-to-Outside: 

If the tool stayed at the center, plunged down, and began cutting outward, the geometry flips. To maintain the same direction of travel, it would switch to Conventional Milling or it would have to reverse its travel direction completely. Conventional milling drags the tool teeth against the metal before cutting, generating immense friction, heat, and a poor surface finish.

To keep the cutting style consistent use always Climb Milling. PowerMill prefers to reset the tool's position back to the ideal starting edge for every single layer.


2. There is danger of plunging into solid metal at the center. When the tool finishes Layer 1 at the center, it leaves a closed pocket floor beneath it. If you tell the tool to plunge straight down into Layer 2 at the center, the bottom of the endmill acts like a flat drill. Endmills are terrible at drilling straight down. Chips get trapped underneath the tool, heat spikes instantly, and the tool can easily snap.

By using a Link to move back outside the pocket, the tool can safely enter the next layer in open air (or use a smooth ramp/helix) where it has room to breathe, and then slice into the material sideways.


3. When cutting from the outside in, the tool path gets smaller and more controlled. If a tool cuts from the inside out: The tool is constantly burying itself deeper into a corner as the boundary expands.
Managing the radial engagement i.e. how much of the tool diameter is cutting metal becomes incredibly chaotic for the software to calculate cleanly, increasing the risk of the tool grabbing too much material and breaking.

What if you REALLY want to stay down?

If your goal is to eliminate that link entirely because you hate watching the tool lift and fly back outside, PowerMill has a specific option for this inside the Area Clearance settings:

You can change the setting from Offset Model to Spiral.

When using a continuous 3D spiral or choosing a bidirectional option, PowerMill will alternate paths where possible, or use a Z-Ramp Lead-in at the center to smoothly corkscrew down into the next layer without lifting. However, it still has to restructure the toolpath coordinates carefully to ensure it doesn't accidentally rub the material the wrong way.