Machine Design #24: What Is an Undercut? How to Recognize, Machine and Avoid Cost Increases

In mechanical drawings, the word undercut is used quite broadly. Some use it to mean a tool relief groove at a shaft shoulder, some use it to talk about a recess that an ordinary end mill cannot reach, and in plastic mold design, an undercut is a shape that prevents the product from being ejected in the mold-opening direction.

If you do not clearly identify which field you are talking about, the same word can lead to three completely different interpretations:

an intentional shape to create a function;
a region that is hard or impossible to machine by the standard method;
a defect that must be removed, like an undercut in a weld.

So when discussing with a machining shop, you should not just write a generic "there is an undercut". The designer needs to clarify:

where the undercut is;
what it is used for;
the approach direction of the tool or the mold-removal direction;
the size and tolerance to be controlled;
which surfaces truly have a function;
whether structural changes or splitting the part are allowed.

This article focuses on the cases machine designers most commonly meet: machining, mold design, tool relief grooves, assembly structures and welding defects.

1. Understanding the true nature of an undercut

1.1. The practical definition in design and manufacturing

In mechanical manufacturing, an undercut can be understood as:

A geometric region hidden or recessed behind a surface, which prevents a tool, electrode, mold or standard implement from accessing or withdrawing in an ordinary direction of motion.

The important point is not whether the part "has a groove" or "has a recess", but the ability to access and withdraw.

For example:

A round groove on a shaft that can be turned with an ordinary grooving tool is not necessarily a hard-to-machine undercut.
A cavity behind a vertical wall, which an end mill cannot reach, is an undercut in milling.
A plastic hook obstructing the mold-opening direction is an undercut in injection molding.
A tool relief groove at a thread root is usually called an undercut or relief groove, but its purpose is to create clearance for the tool and ensure the functional surface runs the full length.

Therefore, when reading a drawing or in technical discussion, you should ask immediately:

Is the undercut in the sense of shape, in the sense of machining technology, or in the sense of a defect?

2. An undercut is not always bad design

An undercut usually raises the cost, but you cannot conclude that every undercut should be removed.

Many mechanisms only work when there is a recessed shape, hook or special groove.

2.1. Common applications

Application	Role of the undercut	Design note
Retaining-ring groove	Holds a part axially	Check the groove width, root diameter, corner radius and the strength of the remaining section
O-ring groove	Holds the sealing element and controls compression	Not every O-ring groove is a hard-to-machine undercut; consider the machining direction and groove position
Snap-fit	Creates an elastic locking hook without screws	Check the deformation during assembly, the material's allowable elongation and the number of insertion/removal cycles
T-slot	Clamps and locates a part	Usually needs a dedicated T-slot cutter, harder chip evacuation than a straight groove
Dovetail groove	Guiding or mechanical locking	Needs a dovetail cutter, control of the angle and mouth size of the groove
Tool relief groove at a shaft shoulder	Lets the tool run the full stroke, avoiding interference with the corner radius	Choose per the standard or the actual fit requirement
Cross holes, internal cavities	Create oil/air passages or a locking mechanism	May need cross-drilling, EDM, 5-axis or splitting the part
Hooks, retaining ridges in a plastic product	Create an assembly function	May require the mold to have a slide, lifter or removable core

2.2. Do not call every groove an undercut

Some naming in practice easily causes confusion:

A keyway is a key groove; it is not always considered an undercut.
An O-ring groove is a sealing groove; it only becomes an undercut in the technological sense when the position or machining direction makes the standard tool hard to access.
A relief groove is a relief; this is a form of intentional undercut, but you must specify the standard and function.
An ordinary pocket is not necessarily an undercut if the tool can enter directly.

The right name helps the machining shop immediately understand the method and the necessary cost.

3. Undercut in machining

3.1. The core issue is the tool's ability to access

In 3-axis milling, the tool usually approaches from above. If the region to be cut is behind a wall or below a protruding edge, an ordinary end mill cannot reach it without hitting the tool shank, holder or spindle.

This is a typical undercut in machining.

Common causes:

an outer wall hides the region to be cut;
the cavity depth is greater than the working length of the tool;
the tool neck is too large;
the designed corner radius is smaller than the available tool radius;
the holder hits the part before the cutting edge reaches the position;
the region to be cut is only accessible from the side or from the rear.

3.2. Commonly used machining methods

T-slot cutter

Used to machine T-slots or grooves with a base wider than the mouth.

Advantages:

common;
suits standard grooves;
lower cost than 5-axis or EDM if the shape is simple.

Limitations:

small tool neck, low rigidity;
hard chip evacuation;
prone to vibration when the tool overhang is large;
unsuitable for deep cavities or very small radii.

Dovetail cutter

Used for grooves with an inclined face or dovetail guide mechanisms.

Must control:

the tool angle;
the depth of cut;
the mouth width;
the wear of the cutting edge;
the measurement method after machining.

Lollipop cutter or undercut cutter

Used to cut a region behind an edge or on a concave curved surface.

The advantage is that it can access a hidden region, but:

the rigidity is usually low;
the tool neck easily collides;
the toolpath is complex;
the machining time is long;
careful CAM simulation is required.

5-axis machining

A 5-axis machine can tilt the tool or the table to create a suitable approach direction.

However, 5-axis does not automatically turn every undercut into an easy-to-machine shape. You still have to check:

whether the holder collides;
whether the tool length is enough;
whether the tilt angle exceeds the machine limit;
whether the fixture obstructs;
the rigidity when the tool is tilted;
the accumulated error of multiple axes;
the cost of programming, set-up and inspection.

EDM

EDM suits when:

the material is heat-treated;
deep cavities, small corners;
complex shapes;
an ordinary cutting tool cannot access;
a precise profile is required.

You can use:

Wire EDM for through-cut profiles;
Sinker EDM for cavities or non-through profiles.

Drawbacks:

long machining time;
an electrode must be made for sinker EDM;
there is a recast surface layer from the discharge;
higher cost than ordinary cutting methods.

3.3. Factors that raise the cost sharply

An undercut usually raises cost not just because of the "strange shape", but because it drags in many secondary operations:

having to change the machine;
having to use a dedicated tool;
having to re-fixture many times;
needing complex CAM;
needing collision simulation;
having to reduce the cutting speed;
hard chip evacuation;
hard inspection;
increased risk of tool breakage;
increased set-up time;
possibly having to order a special tool.

So a small undercut on a drawing sometimes raises the part cost more than expected.

4. Tool relief grooves on shafts and threads

4.1. Why a tool relief groove is needed

When turning a shaft shoulder, cutting a thread or grinding a surface near a shoulder, the tool cannot create an absolutely perfect right angle at the end position. The tool needs run-out clearance, otherwise:

the thread does not have enough usable length;
the bearing shoulder does not seat flush;
the mating part interferes with the corner radius;
the tool is overloaded at the stopping point;
the end-of-stroke surface can be scratched or the wrong size.

A tool relief groove is added to solve this problem.

4.2. Do not choose the size by feel

The groove size needs to suit:

the shaft diameter;
the tool type;
the thread pitch;
the adjacent mating part;
the chamfer radius of the bearing, bush or hub;
the fatigue-strength requirement;
the applicable design standard.

If the groove is too small:

the tool cannot fully clear;
the mating part still interferes;
the functional surface does not have enough length.

If the groove is too deep or the corner too sharp:

the shaft section is reduced;
the stress concentration increases;
fatigue cracking at the shaft shoulder becomes likely.

4.3. Check the corner radius and the mating part

When designing a shaft shoulder fitting a bearing or hub, you must check simultaneously:

the shaft shoulder corner radius;
the radius or chamfer of the mating part;
the shoulder height;
the relief groove diameter;
the groove width;
the machinability and inspectability.

You should not just write "undercut" without a detail section or a reference standard.

5. Undercut in injection mold design

5.1. The definition by mold-removal direction

In an injection mold, an undercut is a shape feature that obstructs the product from being ejected in the main mold-opening direction.

Common examples:

cross holes;
snap-fit hooks;
retaining ridges on a side face;
internal recessed grooves;
cross threads;
a bulge behind a wall;
holes or cavities not aligned with the core and cavity direction.

Without a mechanism to handle them, the product can:

be impossible to eject;
be torn;
deform;
develop white marks;
crack at the hook root;
damage the mold or the ejector pins.

5.2. Solutions in the mold

Solution	Suitable case	Effect
Slide core	External undercut or cross hole	Increases mold size, number of parts and maintenance
Lifter / inclined core	Internal undercut	Needs enough lifting stroke and escape space
Collapsible core	Internal thread or ring ridge	Complex mechanism, high cost
Unscrewing mechanism	Internal or external thread needing rotation to remove	Longer cycle, complex control
Removable insert	Low volume or simple undercut	Costs manual operation
Forced demolding	Small undercut, sufficiently elastic material	Must calculate deformation and stress carefully
Re-split the parting line	Can change the mold-opening direction	Usually a good solution if it does not affect appearance
Change the product shape	When the function allows	Can strongly reduce mold cost and risk

5.3. Undercut ratio in forced demolding

For an elastic plastic product, some small undercuts can be forcibly demolded without a slide.

However, you should not use one general number for every material.

The forced-demolding capability depends on:

the plastic type;
with or without reinforcing fiber;
the elongation at break;
the wall thickness;
the product temperature at demolding;
the hook shape;
the hook root radius;
the deformation length;
the ejection speed;
the number of insertion/removal cycles over the product life.

A commonly used way to express it is:

Undercut ratio (%) = (D - d) / D × 100

Where:

D: the largest size that must pass through during removal;
d: the size at the neck or exit mouth.

The definition can differ per each material maker's documentation. So when using figures for actual design, you must compare against the correct material documentation and part structure.

5.4. DFM before finalizing the shape

Before accepting a slide or lifter, you should check:

whether the mold-opening direction can be changed;
whether the undercut can be brought onto the parting line;
whether a clearance can be added for an elastic hook;
whether the product can be split into two parts;
whether the hook can be replaced with a screw, pin or insert;
whether the volume is large enough to justify the cost of a complex mold;
whether the slide mechanism affects the cooling lines;
whether the slide position weakens the mold or makes it hard to maintain.

In many projects, a small change to the product can significantly reduce the mold cost and mold-trial time.

6. Undercut in welding is a defect

In welding, an undercut is not a functional shape but a groove eaten into at the weld toe, where the base metal is melted but not filled by the weld metal.

6.1. Why it is dangerous

An undercut groove creates:

a reduced load-bearing section;
a stress-concentration point;
a starting point for a fatigue crack;
a risk of local corrosion;
reduced strength of a vibration-loaded structure.

For machine frames, supports, welded bases and cyclically loaded structures, an undercut can be dangerous even if the weld looks continuous from the outside.

6.2. Common causes

welding current too high;
welding speed too fast;
unsuitable torch angle;
arc length too long;
incorrect weaving technique;
uneven heat distribution;
unsuitable joint edge preparation;
poor stopping technique at the weld toe.

6.3. Inspection and acceptance criteria

The allowable limit depends on:

the applicable welding standard;
the type of structure;
the load direction;
static or fatigue load;
the material thickness;
the weld quality level;
the customer's requirement.

You should not take one value like 0.3 mm and apply it generally to every product. The drawing or inspection standard must specify the acceptance criteria.

7. Distinguishing undercut from overcut

These two words are not always a complete antonym pair.

In machining in general:

Undercut can mean a hidden recessed region or a region that has not reached the required shape.
Overcut usually means cutting over size or removing too much material.

In EDM, overcut can also mean the difference in size between the electrode and the machined cavity due to the discharge gap. This is a value that must be accounted for when designing the electrode, not necessarily a defect.

So when writing an NG report or a mold-repair request, you should add a quantitative description:

how much is missing;
how much is excess;
at which position it deviates;
compared to which nominal size or CAD profile;
what the measurement method is.

8. Is there a common standard for undercut size?

There is no single undercut size used across every field.

8.1. In mechanical drawings

Standards like JIS, ISO or internal standards can specify:

undefined edges;
tool relief grooves;
relief for threads;
corner radii;
general requirements for edge breaking;
surface symbols.

However, the designer still has to choose the right standard for each type of shape. You should not just write one general note and expect the machining shop to guess.

8.2. In injection molding

The undercut limit must be taken from:

material data;
the plastic maker's design guide;
deformation simulation;
mold experience;
actual testing.

Unreinforced plastic and glass-fiber-reinforced plastic have very different forced-demolding capabilities.

8.3. In welding

The defect limit depends on the weld quality standard and the type of structure. Fatigue-loaded structures are usually stricter than static-loaded structures.

9. Common undercut design mistakes

9.1. Only checking on the 3D model without thinking about the tool

A CAD model that can be built does not mean it can be machined.

You need to check:

the tool diameter;
the cutting-edge length;
the tool neck length;
the holder size;
the fixturing direction;
the number of re-fixturings;
the tool run-out path;
the inspectability.

9.2. Using too small a corner radius

A small radius can force the shop to use:

a very small tool;
EDM;
many machining steps;
a low cutting speed;
a long polishing time.

If the surface has no special function, you should increase the radius to a level a standard tool can machine stably.

9.3. Designing a deep cavity but too narrow a mouth

A deep cavity and narrow mouth cause:

a weak tool;
hard chip evacuation;
increased vibration;
difficulty getting coolant in;
difficulty measuring the cavity bottom;
increased risk of holder collision.

9.4. Not considering demoldability

A small plastic hook can force the mold to add a slide. The cost increases not only in mold making but also in:

maintenance;
cycle time;
risk of the slide jamming;
cooling layout limits;
increased mold size;
increased number of replacement parts.

9.5. Not specifying the functional surface

If the entire undercut is required to have a tight tolerance and low roughness, the cost will rise sharply.

You should distinguish:

the sealing surface;
the guiding surface;
the clamping surface;
the surface that only needs tool clearance;
the non-functional surface.

9.6. Forgetting to check the strength at the groove root

A relief groove, retaining-ring groove or locking groove all reduce the section. If it bears a cyclic load, you must check:

the nominal stress;
the stress-concentration factor;
the groove root radius;
the roughness;
the heat treatment;
circumferential scratches;
combined bending and torsional load.

10. How to reduce cost from the design stage

10.1. Open an access path for the tool

You can:

make the cavity through;
add a process hole;
widen the cavity mouth;
change the machining direction;
remove unnecessary walls;
allow machining from the opposite face.

A process hole must be evaluated for tightness, stiffness and appearance before applying.

10.2. Split one complex part into several simple parts

Splitting the part is usually effective when:

the undercut is very deep;
5-axis or EDM must be used;
the part is large but the complex region is very small;
it can be located by pins and bolted;
the joint does not affect stiffness or tightness.

However, you should not split just to reduce machining cost while ignoring:

assembly error;
the number of parts;
assembly time;
stiffness;
anti-loosening;
maintenance;
inventory.

10.3. Use standard parts

Some shapes can be replaced with:

a retaining ring;
a lock nut;
a stop bush;
an insert;
a pin;
a bolted cover;
an aluminum profile with a standard T-slot.

10.4. Allow standard tools

Discuss with the machining shop to know:

common tool diameters;
tool nose radii;
standard tool lengths;
available T-slot cutter sizes;
machine limits;
the tolerance that can be achieved stably.

A small change to the radius or groove width can eliminate a special-order tool.

11. How to note an undercut on the drawing

You should not write only the word "UNDERCUT" with an arrow.

You should show fully:

an enlarged section;
the diameter or width;
the depth;
the radius;
the angle;
the tolerance;
the roughness if it has a function;
the relief-groove standard if applicable;
the region where burrs are not allowed;
the edge-breaking requirement;
the machining direction or mold-removal direction when needed;
the inspection requirement by gauge, CMM or optical measuring equipment.

Example notes:

Tool relief groove per the applicable standard.
No burrs at the bearing mounting edge.
Surface A is a functional surface, Ra 1.6.
The groove size must not intrude into the fitting region Ø...

Actual notes must be adjusted per the specific standard and structure.

12. Checklist for the designer

Before finalizing the 3D model

The function the undercut is used to create is clearly identified.
It has been checked whether the undercut can be removed while keeping the function.
The machining direction or mold-opening direction is identified.
It has been checked that the tool, holder, spindle or mold can access.
Chip evacuation and cooling ability have been checked.
The remaining section has been checked to be strong enough.
The corner radius and stress concentration have been checked.
The functional surface has been distinguished from the surface only for tool clearance.
The measurement method is identified.
DFM has been discussed with the machining shop or mold maker.

For a machined part

Whether a standard tool can be used or a special tool must be ordered.
Whether a 5-axis machine, EDM or multiple fixturings are needed.
Whether the tool length reduces rigidity.
Whether the holder risks collision.
Whether the tolerance and roughness are truly necessary.
Whether a process hole can be added or the part split.
Whether the tool relief groove follows a suitable standard.
Whether the corner radius is compatible with the mating part.

For an injection-molded product

The mold-removal direction is precisely identified.
Every cross hole, hook and side ridge has been checked.
Whether the parting line can be changed to remove the undercut.
Whether a slide, lifter or unscrewing mechanism is needed.
Whether it can be forcibly demolded without exceeding the material's deformation limit.
White marks, hook-root cracking and deformation have been checked.
Whether the mold mechanism affects the cooling lines and cycle time.
Whether the volume suits the mold investment level.

For a welded structure

The drawing has specified the weld quality standard.
The fatigue-loaded positions are identified.
The undercut at the weld toe has been checked.
The acceptance criteria are not one value used for every structure.
There is a plan for visual inspection or NDT when needed.

13. Conclusion

An undercut is not a single shape and is not always a defect.

In machine design, you need to clearly distinguish:

undercut in machining: a region a standard tool cannot easily access;
undercut in a mold: a shape obstructing product removal;
undercut as a relief groove: an intentional shape so the tool or mating part does not interfere;
undercut in welding: a defect at the weld toe to be controlled.

The common point is that an undercut is always directly related to the direction of motion, the ability to access and the manufacturability.

A part can look very simple on CAD, but just one small undercut region can completely change the machining method, the mold structure, the fabrication time and the inspection method.

Before releasing the drawing, the designer should ask:

Is this shape truly needed?
In which direction will the tool or mold access?
Is there a simpler alternative?
Which part needs a tight tolerance and roughness?
How will the machining shop inspect it?
Is the additional cost proportional to the function gained?

Understanding the undercut from a manufacturing perspective helps avoid many cases of "CAD can do it but the shop cannot", and significantly reduces drawing revisions, alternative changes and cost overruns after ordering.

View all MINATA technical articles