Shenzhen Alu Rapid Prototype Precision Co., Ltd.
Industry News
CNC Undercut Machining: Design, Tooling and Inspection Guide
CNC undercut machining creates recessed features that a conventional straight end mill cannot reach from the obvious tool direction. These features appear below a shoulder, behind a wall, inside a bore or on the back side of an accessible edge. They may retain a ring, provide tool clearance, form a dovetail, create a sealing relief or satisfy an assembly requirement.
Undercuts are machinable, but they deserve early design review. The cutting head must reach the hidden surface while the neck, shank and holder avoid the surrounding part. A feature that is easy to model may require a fragile long-reach cutter, a second setup, five-axis motion, electrical discharge machining or a custom form tool.
This guide explains undercut types, design-for-manufacturing rules, cutter selection, three-axis and five-axis strategies, turning operations, tolerance and surface-finish control, inspection methods, common defects, cost drivers and the information to include in an RFQ.
What Is a CNC Undercut?
An undercut is a recessed surface that is partly blocked from a straight line of access along the primary spindle direction. The cutter must reach around, below or behind adjacent geometry.
Common examples include:
T-slots and keyseats.
Dovetail grooves.
Retaining-ring grooves.
Relief grooves at shoulders.
Back-side chamfers and deburred cross holes.
Recesses beneath a flange or lip.
Internal grooves in bores.
Hook-shaped, spherical or freeform recessed surfaces.
Tool-clearance features next to threads or bearing seats.
An undercut should not be confused with every narrow or deep pocket. A deep pocket may still be visible to a standard end mill from above. The defining issue is hidden access: part geometry blocks a normal cylindrical cutter, shank or holder.
Why Undercuts Need Special Planning
The cutting edge is only one part of the tool assembly. A successful toolpath must provide clearance for:
The cutter head.
Reduced neck.
Tool shank.
Collet, chuck or holder.
Spindle nose.
Uncut stock and fixtures.
Autodesk's official guidance on machining undercuts identifies lollipop, disc, barrel and dovetail tools as suitable choices for three-axis undercut machining. It also explains that five-axis motion can tilt the tool and reach more areas with a wider range of cutter shapes.
The important lesson is that visible cutter access is not enough. A small head on a long neck may enter the feature, while the holder collides with the part or the neck deflects before the cutter reaches full depth.
Common Types of Machined Undercuts
T-Slots
A T-slot normally begins with a straight access slot. A T-slot or keyseat cutter then enters the slot and removes material laterally below the top opening.
The access slot must be wide enough for the cutter neck and must allow chip evacuation. If the lower width is much larger than the opening, several radial passes may be required rather than one full-width cut.
Keyseats and Woodruff-Key Seats
Keyseat cutters create a controlled-width recess in a shaft, bore or face. Tool diameter, width, corner form and neck length determine the resulting geometry.
Harvey Tool's official keyseat cutter information describes square, corner-radius, full-radius, retaining-ring and staggered-tooth styles. The exact cutter must match the drawing and key or retaining-ring standard.
Dovetail Grooves
Dovetails contain angled walls that mechanically retain a mating component. The included angle, opening width, bottom width, depth and corner radii must be coordinated with a standard or custom cutter.
A dovetail tool can form the sloped surface and nearby features efficiently after the access area has been cleared. Autodesk notes in its dovetail tool guidance that the conical tool surface can machine an undercut more simply than a series of small tools.
Retaining-Ring Grooves
Retaining-ring grooves may be external on a shaft or internal in a bore. The groove width, diameter, bottom radius and edge condition affect ring seating and retention.
Use the applicable retaining-ring standard and specified ring part number. Do not substitute a generic groove based only on nominal shaft or bore diameter.
Shoulder Relief Grooves
Relief grooves provide clearance for grinding wheels, mating component radii, thread runout or bearing shoulders. They are often turned with a grooving or profiling insert.
The relief shape may have a defined radius, width and depth. If a drawing references a standard relief form, identify the standard and edition rather than replacing it with an approximate sketch.
Back-Side Chamfers and Deburring
A lollipop or back-chamfer tool can break a hidden edge after drilling or milling. Examples include the lower edge of a through hole, the reverse edge of a slot and intersections between internal passages.
This operation can remove a secondary manual deburring step, but the design must define chamfer size or edge-break limits. “Deburr” alone may not control a functional edge.
Freeform Undercut Surfaces
Impellers, housings, molds, medical parts and aerospace components may contain curved surfaces hidden behind adjacent geometry. These features often need a lollipop cutter, swarf toolpath, indexed setup or simultaneous five-axis motion.
Can the Undercut Be Removed From the Design?
The most cost-effective undercut is often the one that is redesigned.
Before specifying special tooling, ask:
Can the feature open to an outside edge?
Can the part be split into two components and assembled?
Can a bolted cover or insert create the retaining geometry?
Can the lip become a straight shoulder?
Can the groove use a standard cutter size?
Can the hidden chamfer be replaced with an allowed edge break?
Can a second setup provide direct tool access?
Can the mating component be redesigned instead?
Redesign is not always appropriate. A T-slot, snap feature, sealing relief or retaining-ring groove may be essential. The goal is to keep functional undercuts and remove accidental ones.
Design Rules for CNC Undercuts
Provide a Clear Entry Path
The cutter head and neck must enter the feature. A disc-shaped cutter cannot pass through an opening narrower than its neck, and a dovetail tool needs sufficient axial and radial approach space.
Show the intended entry direction in the CAD model or drawing when it is not obvious.
Use Standard Cutter Geometry
Standard cutter diameter, width, angle, radius and neck length reduce lead time and cost. A custom tool may be justified in production, but it adds procurement time, inspection requirements and replacement risk.
Designers should consult available tool catalogs before finalizing the feature. A small dimensional change can turn a custom undercut into a standard machining operation.
Allow Neck and Shank Clearance
The cutter neck must pass adjacent walls without rubbing. Include positional tolerance, spindle runout, tool deflection and holder clearance—not only nominal CAD clearance.
If the neck is almost the same size as the opening, normal variation can cause contact and tool breakage.
Avoid Unnecessary Reach
Long reach and small neck diameter reduce rigidity. Move the undercut closer to an accessible surface when possible. Increase the access opening or reduce the required lateral reach.
Tool suppliers commonly adjust recommended feeds for the ratio between neck length and neck diameter. Harvey Tool's undercutting end mill guide offers standard, miniature and reduced-shank lollipop-style options, illustrating how reach and neck geometry are central to the application.
Add Practical Internal Radii
Sharp internal corners are usually not produced by ordinary milling. The cutter profile leaves a radius, and a larger radius improves tool strength.
Specify the maximum acceptable radius when clearance is functional. Avoid a zero-radius CAD corner unless the manufacturing method genuinely requires and supports it.
Dimension the Functional Surfaces
An undercut drawing should control the surfaces that affect assembly or performance. Depending on the feature, include:
Groove or slot width.
Undercut depth.
Major and minor diameter.
Included angle.
Radial reach.
Axial location from a datum.
Bottom and corner radii.
Flatness, profile, runout or concentricity.
Surface texture and edge condition.
Do not rely on the 3D model alone for a critical hidden feature.
Specify One-Sided Tolerances When Appropriate
Clearance features sometimes need only a minimum depth or width. A bilateral tight tolerance may increase tool and inspection cost without improving function.
For retaining or locating features, fit may require tighter control. Base the tolerance on the mating part and assembly analysis.
Undercut Cutting Tools
Lollipop Cutters
A lollipop cutter has a spherical or partially spherical head on a reduced neck. It can reach below an edge, contour a hidden surface and deburr back-side geometry.
Important selection variables include:
Head diameter.
Neck diameter.
Neck length.
Wrap angle.
Flute count.
Reach from the holder.
Coating and substrate.
Center-cutting capability, if relevant.
A larger wrap angle reaches farther around the back of a feature but may reduce neck strength or chip space. Confirm the manufacturer's tool model rather than representing it as a generic ball end mill.
Keyseat and T-Slot Cutters
These tools have a disc-shaped cutting head and narrower neck. They produce controlled-width slots and grooves.
Harvey Tool's square keyseat cutter page shows how cutter diameter, cutter width, neck diameter, neck length and radial depth of cut are separate selection variables.
Corner-radius cutters improve edge strength and leave a defined root radius. Staggered teeth may improve shearing action and chip control.
Dovetail Cutters
Dovetail cutters have angled cutting edges. Standard included angles are common, but the cutter's actual geometry and corner form must match the specification.
The access pocket is normally rough-machined first with a straight tool. The dovetail cutter then finishes the angled walls and undercut.
Back-Chamfer Cutters
Back-chamfer tools reach through a hole or slot and cut the far-side edge. They may have a defined angle or curved profile.
Tool diameter must pass through the opening, while the cutting edge must reach the target chamfer. Cross-hole intersections require collision and burr review.
Grooving and Profiling Inserts
On a CNC lathe or mill-turn machine, external and internal undercuts can be machined with grooving inserts, round inserts or profiling tools.
Insert shape, holder hand, approach angle and bar diameter affect access. Internal tools must clear the bore and shoulder while resisting chatter.
Custom Form Tools
A custom form cutter can create multiple surfaces in one pass. It may reduce cycle time in production but increases:
Tool cost and lead time.
Regrind control.
Tool-profile inspection.
Cutting load.
Risk of chatter.
Dependence on one supplier.
For prototypes, several standard tools are often more economical. For stable production, a custom tool may be justified by cycle-time savings.
Three-Axis Undercut Machining
Three-axis machining keeps the tool axis fixed. The cutter shape reaches below or behind adjacent geometry.
A typical sequence is:
Rough the open pocket, bore or access slot with a standard tool.
Remove as much material as possible before using the undercut cutter.
Enter through the access opening with verified clearance.
Rough the undercut in controlled axial or radial passes.
Leave stock for a finish pass.
Finish the functional surfaces with consistent engagement.
Deburr and inspect the hidden edges.
Three-axis machining is economical when a standard special-profile tool can reach the entire feature. It becomes difficult when walls block the shank or the recessed surface changes orientation.
Indexed 3+2 Machining
In indexed machining, the machine rotates the part or tool to a fixed orientation and then cuts using three linear axes. This can expose an undercut directly or shorten tool reach.
Benefits include:
More rigid tools.
Simpler toolpaths than simultaneous five-axis motion.
Better surface consistency.
Fewer manual setups.
Improved access to several sides.
The tradeoff is repositioning accuracy. Datum strategy, rotary-axis calibration and workholding affect feature location between orientations.
Simultaneous Five-Axis Undercut Machining
Five-axis motion changes tool orientation during cutting. It can tilt a standard ball-nose or barrel tool toward hidden surfaces, maintain a better contact point and avoid surrounding walls.
Autodesk's undercut guidance explains that five-axis motion can reach more areas in one operation and broaden the usable tool selection. This can reduce setups and programming duplication.
Five-axis is not automatically cheaper. It requires:
Suitable machine travel and rotary limits.
Accurate kinematics.
Collision-aware CAM.
Verified posts and simulation.
Skilled programming and setup.
Stable workholding.
Use it when the access benefit outweighs programming and machine-hour cost.
Turning Internal and External Undercuts
Rotationally symmetric undercuts are commonly produced on CNC lathes.
External Undercuts
An external groove or relief near a shoulder is accessible with a grooving insert. The tool can plunge, profile or combine axial and radial motion.
Internal Undercuts
Internal grooves require a boring-bar-style tool. The bar must enter the bore, reach behind the shoulder and clear the opposite wall.
Internal operations are more sensitive to:
Minimum bore diameter.
Bar overhang.
Insert width.
Chip evacuation.
Coolant delivery.
Visibility and setup verification.
Autodesk's turning undercut documentation specifically highlights clearance between the back of the insert or holder and the model. That clearance should be verified in CAM and at the machine.
Toolpath Planning
Rough With a Rigid Tool First
Do not ask a slender undercut cutter to remove stock that a standard end mill can remove safely. Open the access region and rough the visible volume first.
Limit Radial Engagement
A disc or lollipop cutter can engage a wide arc. Excessive engagement raises cutting force and can trap chips. Use multiple passes appropriate to the cutter and material.
Use Smooth Entry and Exit
Abrupt entry into full engagement shocks the tool. Roll-in, ramped or tangential moves can reduce the load spike when geometry permits.
Separate Roughing and Finishing
Roughing tool deflection may taper the groove or leave variable stock. A light, consistent finish pass improves size and surface texture.
Control Cutter Compensation
Wear compensation is useful for groove width and diameter, but the control strategy depends on the CAM path and tool geometry. Record the measured cutter, not only the nominal catalog size.
Verify Rest Material
Hidden stock can remain in corners or beneath a lip. Rest machining and section analysis help confirm that all functional surfaces are cut.
Collision Avoidance and CAM Verification
Undercut operations create high collision risk because the cutting edge is hidden.
The CAM model should include:
Complete cutter geometry.
Neck and shank.
Actual holder and gauge length.
Spindle or head where necessary.
Finished part and remaining stock.
Vise, jaws, clamps and fixture plate.
Rotary table and nearby machine components for five-axis work.
Autodesk's shaft and holder collision documentation describes separate shaft and holder clearances and collision-handling modes. These settings are valuable, but simulation does not replace a controlled first run.
At the machine:
Confirm tool and holder against the setup sheet.
Verify gauge length.
Use safe approach positions.
Run above the part or in single block when appropriate.
Reduce rapid override for the first cycle.
Inspect the tool after initial cuts.
Tool Deflection and Chatter
Undercut cutters often have a reduced neck, which lowers bending stiffness. Deflection can produce:
An undersized or oversized groove.
Tapered walls.
Poor surface finish.
Chatter marks.
Uneven corner radii.
Tool breakage.
Reduce risk by:
Using the shortest practical reach.
Selecting the largest permissible neck diameter.
Increasing access rather than extending the tool.
Reducing radial engagement.
Applying manufacturer starting parameters.
Using a rigid holder with low runout.
Roughing before the long-reach tool enters.
Adding a separate spring or finish pass only when process testing supports it.
Repeated spring passes can rub instead of cut, so they should not substitute for a stable process.
Chip Evacuation and Coolant
The recess that makes an undercut difficult also traps chips.
Chip recutting can damage the finish, increase heat and break a slender tool. Internal grooves and deep T-slots are especially vulnerable.
Possible controls include:
Through-tool or directed coolant.
Air blast where safe and compatible.
Pecking or partial withdrawal.
Alternating roughing directions.
Reduced engagement.
Chip-friendly cutter geometry.
Cleaning between process stages.
Coolant jets must reach the actual cutting zone. A stream aimed at the visible tool shank may not flush the hidden cutter head.
Material Considerations
Aluminum
Aluminum usually permits higher cutting speed, but built-up edge and chip welding can affect small undercut tools. Use sharp geometry, suitable lubrication and sufficient chip space.
Stainless Steel
Stainless steel work hardens and generates heat. Avoid rubbing, weak entry and repeated low-chip-load passes. Rigid tooling and controlled engagement are important.
Titanium
Titanium concentrates heat at the cutting edge. Long-reach undercut tools magnify stability problems. Use conservative engagement, reliable coolant delivery and validated tool data.
Hardened Steel
Tool material, coating and edge preparation must match hardness. A form tool may experience high load across a wide contact area.
Plastics
Plastics can deflect, melt, fuzz or close behind the tool. Sharp cutters, heat control and stable workholding are important. Burr acceptance and measurement temperature should be defined.
Tolerances for Undercut Features
Tolerance should reflect function and measurement capability.
Groove Width
Width may be controlled by cutter thickness, axial toolpath position and runout. Cutter wear and deflection can change the result.
Undercut Depth
Radial depth depends on tool diameter, path radius, datum establishment and deflection. For a hidden internal groove, direct measurement may require a dedicated gauge.
Axial Location
Location from a shoulder or datum affects retaining-ring seating, seal position and assembly clearance. Control the datum surface in the same setup when practical.
Angle and Profile
Dovetails and freeform surfaces may need profile tolerance rather than several disconnected linear dimensions. A defined section view prevents ambiguity.
Concentricity and Runout
Turned grooves on shafts or bores may need runout control relative to a functional bearing or sealing diameter. Machine related features in one setup when possible.
Avoid default tight tolerances on every undercut surface. Hidden nonfunctional clearance can usually accept wider variation than a retaining or locating interface.
Surface Finish and Edge Condition
Surface texture matters when the undercut contacts a seal, ring, bearing, sliding component or adhesive.
Specify:
Roughness parameter and limit when functional.
Measurement direction and accessible evaluation method.
Whether tool marks may follow the groove.
Burr and sharp-edge limits.
Maximum corner radius.
Scratch, chatter and tear acceptance.
Final condition after coating or heat treatment.
A generic surface-finish value does not automatically control waviness, chatter or isolated scratches.
Burr Control
Undercuts are difficult to deburr because both the burr and the tool may be hidden.
Typical burr locations include:
Access-slot edges.
Dovetail lips.
Cross-hole intersections.
Retaining-ring groove edges.
Back-side chamfers.
Entry and exit points of form tools.
Plan deburring during process design. Options include a second cutting pass, back-chamfer tool, abrasive flow, thermal or electrochemical methods, brushing, media, hand tools under magnification or a purpose-made scraper.
The method must not round a functional retaining edge or change groove width.
Coatings and Heat Treatment
Anodizing, plating, PVD coating, nitriding and heat treatment can change undercut dimensions and surface condition.
The drawing should state:
Whether dimensions apply before or after finishing.
Coating thickness and buildup assumptions.
Masked surfaces.
Whether the groove bottom and sidewalls receive coating.
Post-treatment inspection requirements.
A coating can narrow a slot, reduce dovetail clearance or change the fit of a retaining ring. Hidden surfaces may also receive uneven coverage depending on the process.
How to Inspect CNC Undercuts
Dedicated Go/No-Go Gauges
Functional gauges are efficient for repeat production. They can verify access, width, depth or mating-part fit without producing a full dimensional value.
Groove Micrometers and Calipers
Specialized contacts can measure accessible groove width, diameter or location. Confirm that contact geometry reaches the true functional surface.
Bore Gauges and Internal Groove Gauges
Internal retaining-ring grooves may need expanding contacts or dedicated comparative gauges. Master setting and measurement force should be controlled.
CMM With Special Styli
Disc, star, L-shaped or custom styli can reach hidden surfaces. The probe qualification, approach vector and collision clearance must be planned.
Optical and Vision Inspection
Vision systems can inspect visible profiles, tool form and external grooves. Deep internal surfaces may remain hidden.
Contour and Form Measurement
A contour tracer can measure a section through an accessible groove or relief. Stylus access and tracing direction must match the feature.
Replica or Sectioning
For difficult prototype features, a molding replica may allow optical measurement. Destructive sectioning can validate a process during qualification but is usually unsuitable for every production part.
Functional Assembly Check
A mating component, ring, key or slide can verify fit. Functional checks should supplement, not automatically replace, dimensional evidence when traceability is required.
Common Undercut Machining Problems
Tool Breakage at Entry
Possible causes include immediate full engagement, neck contact, incorrect stock model, excessive feed or poor run-in motion.
Groove Too Narrow
Cutter wear, deflection, wrong tool thickness or coating buildup may be responsible. Verify the cutter and final-surface requirement.
Groove Too Wide
Runout, chatter, repeated offset errors or an incorrect cutter can enlarge the feature.
Tapered or Wavy Walls
Long reach, inconsistent engagement, weak workholding or chatter may deflect the tool.
Remaining Stock Under the Lip
The toolpath may not reach the complete hidden surface. Compare the actual cutter envelope with the CAD geometry and use sectioned verification.
Holder or Neck Witness Marks
Insufficient clearance allows a noncutting part of the assembly to rub the workpiece. Stop and correct the tool or path; do not treat the mark as a normal finish condition.
Trapped Burrs
Burrs can prevent ring seating or scratch a mating component. Specify an accessible deburring and inspection method.
Incorrect Dovetail Fit
Angle, tool form, depth, corner radius and coating all affect the effective fit. Inspect the functional profile rather than one opening dimension alone.
Cost Drivers
Undercut machining cost increases with:
Custom cutter geometry.
Long reach and small neck diameter.
Restricted access.
Additional setups or five-axis motion.
Tight groove width, depth or location tolerances.
Difficult internal inspection.
High-performance materials.
Special burr and edge requirements.
Coating compensation.
Low quantity with one-time programming and tooling.
Complex collision verification.
Required CMM reports or functional gauges.
A standard T-slot in accessible aluminum may be straightforward. A deep internal dovetail in hardened steel with tight profile tolerance and no direct inspection path is a different manufacturing problem.
DFM Checklist for Undercuts
Before releasing the design, confirm:
The undercut serves a defined function.
The feature cannot be simplified without losing function.
The entry direction is clear.
A standard cutter can create the profile.
The cutter neck and holder have clearance.
Tool reach is as short as practical.
Internal radii match cutter capability.
Functional surfaces and datums are dimensioned.
Tolerances reflect the mating requirement.
Burr and edge limits are specified.
Coating condition is defined.
An inspection method can reach the feature.
The CAD model includes the complete undercut.
Section views show hidden geometry clearly.
RFQ Checklist for Undercut Parts
Send the CNC supplier:
Native 3D CAD model and controlled 2D drawing.
Material grade and condition.
Prototype and production quantities.
Undercut type and functional purpose.
Entry direction or allowed setups.
Width, depth, diameter, angle and radii.
Datum scheme and critical locations.
Surface finish and edge requirements.
Mating component, key or retaining-ring specification.
Coating, heat treatment and masking.
Final dimensional condition.
Inspection report and gauge requirements.
Any approved standard cutter or tool restriction.
Areas where tool marks are unacceptable.
Annual volume and repeat-order expectations.
For a broader purchasing package, see our CNC Machining RFQ Checklist.
Sample CNC Undercut RFQ
Please quote the attached 7075-T6 aluminum housing in quantities of 5, 50 and 250. The part contains an internal retaining groove and two back-side chamfers. Dimensions apply after Type II anodizing; the retaining groove is masked. Use the specified retaining-ring part number to verify functional fit. Inspect groove width, diameter and axial location, and provide a dimensional report for the first three parts. Burrs are not permitted on the ring seating edges. Alternative standard cutter radii may be proposed before manufacture.
This request identifies the material, quantities, hidden features, coating condition, mating hardware, inspection scope and acceptable DFM discussion.
Frequently Asked Questions
What is an undercut in CNC machining?
It is a recessed feature that cannot be fully reached by a conventional straight cutter from the primary tool direction because adjacent geometry blocks access to the cutting edge, shank or holder.
What tools are used for CNC undercuts?
Common tools include lollipop cutters, T-slot and keyseat cutters, dovetail cutters, back-chamfer tools, grooving inserts, profiling tools and custom form cutters. Selection depends on the feature profile and access.
Can a three-axis CNC machine cut an undercut?
Yes, when a shaped cutter can enter the feature and reach all surfaces without the neck, shank or holder colliding. Complex changing orientations may require indexed or simultaneous five-axis machining.
Why are undercuts expensive?
They can require special cutters, long reach, additional setups, complex CAM verification, slow cutting parameters and difficult inspection. Standardized accessible geometry reduces cost.
Should I use a lollipop cutter or a T-slot cutter?
A lollipop cutter suits curved contouring, hidden surfaces and back-side deburring. A T-slot or keyseat cutter suits controlled-width disc-shaped grooves. The CAD profile and access determine the correct choice.
How much clearance does an undercut tool need?
There is no universal value. Clearance must account for the actual cutter, neck, shank, holder, runout, tool deflection, machine accuracy and tolerance stack. Verify the complete assembly in CAM and at setup.
Can a sharp internal undercut corner be milled?
Ordinary milling leaves a radius based on the cutter profile. EDM or a special process may create a sharper corner, but redesigning for an allowed radius is usually more economical.
How are internal undercuts inspected?
Options include groove gauges, dedicated go/no-go gauges, specialized CMM styli, contour instruments, replicas and functional mating checks. Inspection access should be planned during design.
Does anodizing change an undercut?
Yes. Coating buildup can narrow grooves, change radii and affect mating clearance. State whether dimensions apply before or after coating and define masking.
When is five-axis machining worthwhile?
It is valuable when tool tilting provides access with a shorter or stronger cutter, reduces setups or reaches freeform recessed surfaces that shaped three-axis tools cannot machine efficiently.
Final Recommendations
Reliable CNC undercut machining begins with access analysis. Review the cutter head, neck, shank, holder, stock and fixture—not just the visible cutting edge. Use standard cutter geometry, keep reach short, rough with rigid tools first and simulate the complete tool assembly.
On the drawing, define the functional profile, datum, tolerance, edge condition and final coated state. Plan how the hidden feature will be deburred and measured before production begins. If the feature requires a custom tool or five-axis motion, compare that cost with a design change or alternate assembly.
AluPrototype machines T-slots, dovetails, retaining grooves, reliefs, back-side chamfers and freeform undercuts for prototype and production parts. Explore our CNC machining article library or request a quote with your CAD model, drawing, material, quantities, finish and inspection requirements.