CNC drilling guide

How to Drill an Angle on a CNC Machine

With 16 simultaneous 5-axis machining centers in Dongguan, we drill angled holes every week. This guide shows the setup, workholding and toolpath choices that decide whether an angled hole lands within ±0.005 mm or walks off location. It is written for engineers and programmers who need a working process, not a sales pitch.

Get Instant Quote Talk to an Engineer

±0.005 mm tolerance5-axis drillingDFM in 12 hoursNo MOQ

drill an angle cnc machine setup on a 5-axis center

On this page

Key takeaways

Two ways to drill an angleTilt the tool or tilt the part. On a 3-axis machine you tilt the part; on a 5-axis machine you tilt the tool.

Spot drill firstA 90° spot drill 1–2 mm deep stops the twist drill from walking off location.

Watch the effective rakeOn a tilted entry the drill's cutting edge sees a changed angle. Keep tilt under 30° where possible.

Rigidity beats speedAngled entry loads the drill sideways. Shorten overhang and drop feed 20–30% versus a normal hole.

Basics

What changes when the hole is not square to the spindle

A drill is designed to cut on its point. The moment the axis of the hole is not parallel to the spindle, the point stops engaging evenly. One lip bites first and pushes the drill sideways. That sideways push is what turns a simple hole into a location problem. The stiffer the setup, the smaller the push.

There are only two ways to drill an angle CNC style. You can keep the drill vertical and tilt the part, or you can keep the part flat and tilt the head. A 3-axis machine can only do the first. A 5-axis machine with a rotary table or a swivel head can do the second, and that is usually the better choice for anything with more than one angled hole.

The angle itself matters less than where it sits in the tolerance stack. A 15° hole in a bracket is easy. A 15° hole that must intersect a cross-drilling within 0.1 mm is a different job. Before you program anything, decide which feature is the datum and which one is allowed to move.

1
3-axisTilt the part with an angle plate, sine vise or sine bar. Cheap, but you re-clamp for every angle.
2
4-axisRotary table indexes the part. Good for holes on a single cylindrical face.
3
5-axisTool stays normal to the surface. Best for compound angles and intersecting holes.

Workholding

Workholding for an angled hole

Most angled drilling failures are clamping failures. When the drill enters at an angle, the cutting force has a component that tries to slide the part. A vise that grips a flat face on a square part has plenty of friction. The same vise gripping a 15° face has much less, and the part creeps.

Use a positive stop in addition to friction. A dowel pin, a shoulder bolt or a machined step that the part butts against will take the lateral load. On thin plates, support under the drill exit. A 20 mm thick plate with a 10 mm hole drilled at 45° has a very thin wall at the break-through point, and the drill will push it out.

For a 5-axis setup, the rotary table carries the part. Check the table's clamp torque, not just its positioning accuracy. A table that repeats to 5 arc-seconds but flexes under a 12 mm drill will still throw the hole off. We keep a Ø400 mm rotary table for parts that need it, and we check runout on the part after clamping, not just on the table.

1
Positive stopButt the part against a pin or step so the drill cannot push it sideways.
2
Support the exitBack the break-through side with a sacrificial plate or a fitted support.
3
Check after clampingIndicate the part, not the fixture. Clamping can move a part 0.02 mm.

Tooling

Choosing the drill and the entry point

A standard 118° twist drill is fine for most angled entries up to about 30°. Past that, the point starts to skid on the surface. A 90° spot drill, used 1–2 mm deep, gives the twist drill a cone to sit in and removes most of the walk. Spot with the same angle or steeper than the drill point.

For deep holes, a parabolic-flute drill clears chips better than a standard jobber drill. On a 45° entry into 6061 aluminium, we run a 8 mm carbide drill at 3,000–4,000 rpm and 400–600 mm/min feed, with a 20–30% reduction from the flat-entry feed. In 304 stainless, drop to 800–1,200 rpm and 60–120 mm/min.

Do not use a long drill if a short one will reach. Overhang multiplies the sideways deflection. If the hole is 30 mm deep but only 10 mm of flute is needed to start it, use a stub drill for the entry and a longer drill only after the cone is established. Peck from the start, because chips do not clear well from an angled entry.

1
Spot 1–2 mmEnough to form a cone, not enough to burn the point.
2
Reduce feed 20–30%Applies to the first 2–3 mm of cutting, then return to normal.
3
Peck from the startSmall pecks, 1×D or less, until the full diameter is engaged.

CAM

Programming the toolpath

In CAM, the difference between a good angled hole and a scrapped part is usually the entry move. Plunge straight into the surface along the hole axis. Do not ramp into an angled hole unless the tool is a mill, not a drill. For a drill, the toolpath is a positioning move, a spot, then a drilling cycle.

On a 3-axis machine with the part tilted, the hole axis is no longer parallel to Z. You can drill it with the part tilted and the drill still vertical only if the tilt is small. Past about 10°, the drill will not enter cleanly. The correct 3-axis method is to tilt the part so the hole axis is vertical again, which means re-fixturing for each angle.

On a 5-axis machine, use the rotary axes to bring the hole normal to the spindle. Then the cycle is a normal drilling cycle with the machine's RTCP or TCPM active. If TCPM is off, the posted coordinates will be wrong by the pivot distance. This is the single most common programming error we see in customer files.

1
Plunge, do not rampA drill cuts on its point. A ramp move loads the side of the flutes.
2
Check TCPMWith TCPM off, pivot error scales with the distance from the rotary center.
3
Simulate the entryVerify the spot drill clears the angled surface before the twist drill enters.

Step by step

Step by step: drill an angle CNC machine

1
1. Define the datum and the anglePick the face the hole is measured from. Write the angle and the tolerance. If the angle tolerance is looser than ±0.5°, a sine vise is enough. If it is tighter, plan for a 5-axis setup or a dedicated fixture.
2
2. Choose the setupOne or two holes at a shallow angle: tilt the part on an angle plate or sine vise. Multiple holes or compound angles: use the 5-axis rotary table. Do not tilt a part to 45° on a 3-axis machine and expect the drill to enter cleanly.
3
3. Build the fixtureAdd a positive stop against the drilling direction. Support the exit side. Indicate the part after clamping, not before. If the part moves more than 0.02 mm when you clamp, the fixture is wrong.
4
4. Pick the spot drill and the drill90° spot drill, 1–2 mm deep. Carbide twist drill with the shortest flute length that reaches. For 6061 aluminium: 3,000–4,000 rpm, 400–600 mm/min. For 304 stainless: 800–1,200 rpm, 60–120 mm/min.
5
5. Set the entry parametersReduce feed 20–30% for the first 2–3 mm. Peck at 1×D or less until the full diameter is engaged. Turn coolant on before the drill touches the part, not after.
6
6. Verify the first holeDrill one hole, then check position and angle with a pin gauge or a CMM. Adjust the work offset if needed. Do not run the full batch on an unverified setup.
7
7. Inspect and deburrAngled holes break through with a sharp, elongated edge. Deburr with a countersink or a hand tool. Check the hole diameter at the entry and the exit, because an angled break-through is often larger than the nominal size.

Setup choice

Which setup for which angled hole

Match the setup to the angle, the hole count and the tolerance.

Setup	Best for	Accuracy	Watch out for
Angle plate on 3-axis	Single hole, angle over 15°	±0.05 mm typical	Re-clamping for every angle
Sine vise on 3-axis	Shallow angle, ±0.5° tolerance	±0.02 mm typical	Vise lifts under side load
4-axis rotary table	Holes on one cylindrical face	±0.01 mm typical	Table clamp torque limits
5-axis simultaneous	Compound angles, many holes	±0.005 mm achievable	TCPM must be active
5-axis 3+2 (indexed)	Angled holes, flat-to-flat	±0.005 mm achievable	Indexing time adds cycle time
Right-angle head	Large parts that cannot tilt	±0.02 mm typical	Head rigidity, limited reach

The short version

If you have one angled hole and a 3-axis machine, tilt the part and spot drill. If you have several angled holes, compound angles, or a tolerance tighter than ±0.05 mm, use a 5-axis setup and keep TCPM on.

Get Instant Quote Talk to an Engineer

FAQs

Frequently asked questions

Can I drill an angled hole on a 3-axis machine?

Yes, but you have to tilt the part. The hole axis must end up parallel to the spindle, otherwise the drill skids on the surface.

Tilting the part means re-fixturing for each different angle. For one or two holes this is fine. For a part with six angled holes, a 5-axis setup is faster and more repeatable.

What is the maximum angle a drill can enter without spotting?

In practice, about 5–10° on a flat surface. Past that, the point walks. Spot drilling 1–2 mm with a 90° spot drill extends that to roughly 30°.

Past 30°, the geometry of a standard twist drill works against you. Use a steeper point angle or a dedicated flat-bottom or ball-nose entry.

Why does the hole come out larger than the drill diameter?

The drill is orbiting, not spinning true. Causes are long overhang, a worn drill, a loose chuck or collet, or a part that moves under the side load.

Check runout at the drill tip, not at the holder. Shorten the overhang and re-check the clamp. On an angled break-through, some oversize is normal because the exit edge is thin.

How do I hit an intersecting hole at an angle?

Drill the straight hole first, then the angled one, and use the straight hole as the datum. That way the angled drill breaks into a known cavity and does not wander.

If the intersection is critical, leave 0.2–0.3 mm on the angled hole and ream or mill it to size. A drill is a roughing tool at the point where two holes meet.

Do I need coolant for angled drilling?

Yes, and it should be on before the drill touches the part. Angled entry produces a longer chip and the flutes clear it less efficiently than a flat entry.

Through-spindle coolant helps most on deep holes. On aluminium, air blast plus mist can be enough. On stainless and titanium, use flood or through-tool coolant.

What angle tolerance can a CNC shop hold?

On a 5-axis machine with an indexed setup, ±0.05° on the angle is realistic for a well-fixtured part. Position tolerance is usually the tighter of the two.

On a 3-axis machine with an angle plate, expect ±0.2° to ±0.5° depending on the plate and the clamp. Tell your shop which one matters: the angle or the hole position.

Send us your angled-hole part

Upload a STEP file and we will return a quotation and a free DFM analysis within 12 hours, including a note on the setup we would use for each angled hole.

12-hour quote100% inspectionNDA on request

Get Instant Quote Talk to an Engineer