Every mechanical engineer eventually faces the same moment of realization: the feature you designed with confidence—a pocket with an internal groove, a snap-fit lip, a dovetail slot—can’t be reached by a standard end mill.
That’s the moment you discover undercuts.
Undercuts are features that are inaccessible from a single spindle direction. They require specialty tooling, careful planning, and a solid understanding of what T-slot cutters, dovetail cutters, and lollipop tools can actually do.
But undercuts don’t have to be a roadblock. With the right design rules, they can be machined efficiently and cost-effectively—often without a 5-axis machine.
In this guide, we’ll walk you through everything a mechanical engineer needs to know about designing undercuts for CNC machining: the tooling, the dimensional limits, the design rules, and the common mistakes that cost you time and money.
Explore our CNC machining services for complex geometries including undercuts →
What Is an Undercut in CNC Machining?
An undercut is any feature on a part that cannot be machined with a standard straight-shank cutting tool from the primary spindle axis. In practical terms, it’s a recessed area, groove, or angled surface that is “hidden” from a top-down tool approach.
The key characteristics that make a feature an undercut:
| Feature Attribute | Standard Tool Accessible? | Requires Specialty Undercut Tool? |
|---|---|---|
| Vertical wall | ✅ Yes (end mill from top) | No |
| Hole or through-slot | ✅ Yes | No |
| Internal groove on a bore wall | ❌ No | Yes |
| O-ring groove on a face | ✅ Yes (if shallow and wide) | Sometimes |
| Dovetail slot (angled walls) | ❌ No | Yes |
| T-slot on a side wall | ❌ No | Yes |
| Back-tapered feature | ❌ No | Yes |
| Snap-fit lip or internal undercut | ❌ No | Yes |
Why undercuts matter for cost:
Every undercut feature typically requires a separate tool and an additional setup or operation. This increases machining time and cost. Some undercuts can be incorporated into standard operations if designed correctly; others demand very specific tooling and approach strategies.
This guide is about designing your undercuts so they fall into the first category as often as possible.
1. The Three Types of Undercut Tools (And What They Can Reach)
Before you can design an undercut, you need to understand the tools that cut them. There are three primary types:
T-Slot Cutters
A T-slot cutter has a flat, disc-like cutting head mounted on a smaller-diameter shank. Think of it like a tiny circular saw blade on a stick.
| Characteristic | Typical Range | Design Implication |
|---|---|---|
| Blade Diameter (D) | 12–50 mm (0.5–2.0″) | Determines width of slot |
| Blade Width (W) | 2–15 mm (0.08–0.6″) | Determines height of undercut |
| Shank Diameter (d) | 6–20 mm (0.25–0.8″) | Must fit through access slot |
| Reach Depth | Up to 3–4× blade diameter | Deepest accessible groove depth |
What T-slot cutters are best for: Internal grooves on side walls, T-slot channels, retaining ring grooves, undercut channels for mounting hardware.
Key design constraint: The shank diameter must pass through the access slot. This means your slot width must be greater than the shank diameter, and the shank must be able to reach the undercut location without interference.
Dovetail Cutters
A dovetail cutter has a tapered cutting head, often in the shape of a truncated cone with cutting edges along the angled side. The included angle is typically 45°, 60°, or 90°.
| Characteristic | Typical Range | Design Implication |
|---|---|---|
| Included Angle | 45°, 60°, 90° | Must match designed dovetail angle |
| Tip Diameter | 3–15 mm (0.12–0.6″) | Controls bottom width of slot |
| Cutting Length | 3–12 mm (0.12–0.5″) | Maximum dovetail depth |
| Shank Diameter | 6–16 mm (0.25–0.63″) | Clearance required for approach |
What dovetail cutters are best for: Dovetail slots for sliding assemblies, angled retaining grooves, sealing surfaces in fixtures.
Key design constraint: The dovetail angle you design must match an available cutter angle. Custom angles are possible but expensive. Stick to 45°, 60°, or 90° standard angles whenever possible.
Lollipop (Ball-End Undercut) Cutters
A lollipop cutter (also called a spherical undercut tool) has a spherical or half-spherical cutting head on a necked shank. This is the most versatile undercut tool for curved profiles.
| Characteristic | Typical Range | Design Implication |
|---|---|---|
| Sphere Diameter | 3–20 mm (0.12–0.8″) | Controls fillet radius of undercut profile |
| Neck Diameter | 2–10 mm (0.08–0.4″) | Must be smaller than sphere; determines clearance |
| Reach Length | Up to 5–8× neck diameter | Maximum depth from access point |
What lollipop cutters are best for: Rounded internal grooves, undercuts on contoured surfaces, deburring hard-to-reach edges, transitioning from a side wall to a back-tapered surface.
Learn more about tool selection for complex machining features →
2. Dimensional Design Rules: How to Size Undercut Features
Designing an undercut is fundamentally about respecting the tool’s access path. Every undercut can be described by a few critical dimensions.
General Rule: Access First, Undercut Second
A tool must first enter the part through an existing opening (a hole, slot, or from an edge), then shift laterally to cut the undercut. Your design must accommodate both phases.
Critical dimensional relationships:
| Design Parameter | Rule | Why |
|---|---|---|
| Slot Width (entry) > Shank Diameter | Slot ≥ d_shank + 0.5–1.0 mm clearance | Tool must pass through without rubbing |
| Undercut Depth ≤ Tool Blade/Reach Length | Depth ≤ L_reach | Tool can’t exceed its physical reach |
| Internal Corner Radius of Undercut = Tool Corner Radius | r_internal = r_tool tip | Tool geometry dictates minimum fillet |
| Undercut Height ≥ Tool Blade Width | Height should be at least blade width; multiple passes for taller slots | Single pass is faster; multiple passes add cost |
| Clearance for Tool Entry from Edge | Tool must enter from an edge or a through-slot | Blind undercuts require special strategies |
T-Slot Design Dimensions (Diagram Reference)
[Refer to illustration: A T-slot cross-section with dimensions labeled.]
When designing a T-slot:
- Slot width (S) = desired opening. Must be > shank diameter of chosen T-slot cutter.
- Undercut width (U) = the internal widened area. Determined by blade diameter minus shank diameter, divided by 2 (for symmetrical slots).
- Undercut height (H) = blade width.
- Corner radius (R) = tool tip radius. Typically 0.2–0.8 mm. Specify if you need a sharp corner (requires additional process).
Dovetail Slot Design Dimensions
For a dovetail slot:
- Intersection angle (θ) = 45°, 60°, or 90°. Match a standard cutter.
- Slot bottom width (b1) and top width (b2) are determined by angle and depth.
- Depth (d) limited by cutter’s cutting length.
- Entry must be from the end of the slot (open on at least one side).
Read our DFM analysis guide to ensure your undercut design is manufacturable before quoting →
3. Common Undercut Design Mistakes (And How to Avoid Them)
Mistake #1: Designing a Blind Undercut With No Entry Path
Undercuts require a tool to enter from somewhere—an open edge, a through-slot, or a pre-drilled hole. If the undercut is completely enclosed with no access path larger than the tool’s cutting head, it’s unmachinable.
Solution: Add a through-hole or an open slot on an adjacent surface to allow tool entry. Or split the part into two components that are assembled after machining.
Mistake #2: Ignoring Tool Shank Diameter
The undercut’s entry slot must be wider than the shank diameter, not just the cutting blade. Designers often dimension the slot width based on the blade width, forgetting that the shank must pass through it first.
Solution: When specifying an undercut slot, always check that:
Entry slot width ≥ (shank diameter + 1 mm clearance)
Mistake #3: Specifying Sharp Internal Corners
Undercut tools have a finite tip radius. If you design a zero-radius internal corner on a dovetail or T-slot, it will require a secondary EDM operation or be impossible.
Solution: Allow a radius of at least 0.3 mm (0.012″) for small cutters or 0.5–0.8 mm for standard sizes. Check the tool catalog for your chosen cutter’s tip radius.
Mistake #4: Deep Undercuts With Short Tooling
The reach of an undercut tool is limited by the neck or shank length. A deep internal groove far from the entry point is unreachable with standard tooling. Custom long-reach cutters exist but are fragile and expensive.
Solution: Keep undercut depth within 3–4× the blade or cutter diameter for T-slot and lollipop tools. If you need deeper, consider a 5-axis approach or redesign the part.
Mistake #5: Mixing Undercut Angles
Using multiple dovetail angles on the same part requires tool changes and separate operations. This drives up cost significantly.
Solution: Standardize on one dovetail angle (preferably 60°, the most commonly available) throughout your design.
Learn how factory-direct machining avoids hidden upcharges for complex features →
4. Undercut Machining Strategies: From 3-Axis to 5-Axis
3-Axis Machining of Undercuts
Most undercuts can be machined on a standard 3-axis CNC mill. The key is tool access from the side or through a slot.
Process on a 3-axis machine:
- Mill all accessible features from the top using standard end mills.
- Drill or mill entry holes/slots for undercut tool access.
- Change to undercut tool and enter from the access path.
- Machine the undercut in one or multiple passes.
- If the undercut is on multiple sides, re-fixture the part.
Limitation: Only undercuts with a clear straight-line access path can be machined in 3-axis. Undercuts on curved internal surfaces or angled beyond the tool’s reach require more axes.
5-Axis Machining for Complex Undercuts
With a 5-axis machine, the spindle can tilt, allowing a shorter, more rigid tool to access undercuts from different angles. This eliminates many of the reach and clearance constraints of 3-axis undercut machining.
What 5-axis enables:
- Undercuts on curved surfaces without through-slots.
- Tighter tolerances due to stiffer tool setups.
- Fewer setups—multiple undercuts can be accessed in one operation.
At Baosheng, we combine our 5-axis capability with manual DFM review to optimize the process for your specific part geometry.
Explore our 5-axis CNC machining capabilities →
5. Design Checklist for CNC Undercuts
Use this checklist before finalizing your design:
- Entry path exists: Slot, hole, or open edge with clearance for tool shank.
- Slot width > shank diameter: Verified against tool catalog dimensions.
- Undercut depth within reach: ≤ 4× blade diameter for T-slot; ≤ cutting length for dovetail.
- Angles match standard tooling: 45°, 60°, or 90° dovetail angles.
- Internal radii specified: R ≥ 0.3 mm minimum; larger if possible.
- Single angle per part (if possible): Reduces tool changes.
- Feature is deburrable: Undercut edges should have a small chamfer or radius if deburring access is needed.
- Consider 5-axis alternation: If reach is a problem, can the part benefit from 5-axis access?
Undercut Tooling and Design Limits Quick Reference
| Undercut Type | Tool | Max Reach | Standard Angles | Min Internal Radius | Entry Path Required |
|---|---|---|---|---|---|
| T-Slot | T-slot cutter | 3–4× blade dia. | N/A (straight sides) | 0.3–0.8 mm | Yes (slot or edge) |
| Dovetail | Dovetail cutter | Cutter-specific (3–12 mm) | 45°, 60°, 90° | 0.2–0.5 mm | Yes (open end) |
| Curved Undercut | Lollipop / ball undercut | 5–8× neck dia. | N/A (spherical) | = sphere radius | Yes (hole or slot) |
Need Help With Your Undercut Design?
At Baosheng Industry, we don’t just machine parts—we help engineers design for manufacturability. Our manual DFM review will analyze your undercut geometry and recommend specific tooling strategies to simplify machining and reduce cost.
With 582 CNC machines including 5-axis capability, AS9100D / ISO 13485 / IATF 16949 certifications, and over 20 years of experience, we’re the direct manufacturing partner engineers trust for complex geometries.
Upload your CAD file today. We’ll provide a free DFM analysis within 24 hours with actionable undercut design feedback.
Free DFM Analysis • Undercut Design Feedback • 24-Hour Engineer Response • AS9100D / ISO 13485 / IATF Certified • ITAR Registered • Open to Factory Visits
Frequently Asked Questions (FAQ)
Q1: What is the difference between a T-slot cutter and a dovetail cutter?
Answer: A T-slot cutter has a flat, straight-sided blade used for internal parallel grooves. A dovetail cutter has a tapered, angled cutting profile used for dovetail slots with standard angles of 45°, 60°, or 90°.
Q2: What is the minimum slot width for an undercut feature?
Answer: The minimum slot width must be at least the tool’s shank diameter plus 0.5–1.0 mm clearance. The cutting blade diameter itself is larger, so the slot through which the tool enters must accommodate the shank.
Q3: Can blind undercuts be machined?
Answer: Generally no. An undercut requires a tool to enter from an open edge, a through-slot, or a pre-drilled hole. If the undercut is completely enclosed with no access path, it is unmachinable without alternative process like EDM.
Q4: What standard dovetail angles should I use in my design?
Answer: Standard dovetail cutter angles are 45°, 60°, and 90°. 60° is the most commonly available and is recommended for general-purpose use. Custom angles are possible but increase cost.
Q5: How deep can a T-slot undercut be?
Answer: Typically, the depth of a T-slot is limited to 3–4 times the blade diameter of the cutter. Deeper features require custom long-reach cutters, which are fragile and expensive.
Q6: Does adding undercuts increase machining cost significantly?
Answer: Yes, undercuts generally require specialty tooling, additional setups, or longer cycle times, which increases cost. However, by following design best practices—standard angles, adequate access paths, reasonable depths—you can minimize the cost impact.
Q7: Can 5-axis CNC eliminate the need for undercut tooling?
Answer: In many cases, yes. 5-axis machining allows the spindle to tilt and reach undercut areas with standard, shorter tools, often eliminating the need for specialty cutters and reducing cycle time. However, some features still benefit from dedicated undercut tooling.
Q8: What should I include in my CAD model to help the machinist with undercuts?
Answer: Clearly specify the undercut profile, angle, depth, and any required corner radii. If the part has multiple undercut orientations, consider adding a note or 3D view annotation indicating access path expectations. Our DFM review will catch any issues early—upload your CAD and we’ll provide feedback.
Continue Reading
- DFM Analysis: Why Automated Software Can’t Replace a Machinist’s Eye
- How to Achieve a Mirror Finish on 6061 Aluminum Without Secondary Polishing
- Machining PEEK vs. PEKK: Tolerances, Speeds, and Feeds Guide for Engineers
- Hidden Costs of Instant CNC Quoting Platforms: What Procurement Managers Need to Know (2026)
