Process guide

How to Machine Bumps CNC: A Step-by-Step Process Guide

Bumps are small raised features used for alignment, contact pads, heat transfer and snap fits. This guide covers the setup, tooling, programming and inspection steps that keep them on size. It is written for engineers and buyers who need to judge whether a bump feature can be machined at all, and what it costs to hold it.

Get Instant Quote Talk to an Engineer

±0.005 mm toleranceRa 0.8–1.6 μm finish1 pc to 10,000+DFM in 12 hours

On this page

Key takeaways

Bumps are a tooling problem, not a programming problemA 0.3 mm raised pad fails because the tool bends, not because the code is wrong.

Keep the tool as short as the geometry allowsDeflection scales with the cube of stick-out length. Every millimeter matters.

Rough the field first, then cut bumpsLeaving 0.1–0.2 mm on the floor lets one finishing pass cut bumps and floor together.

Below Ø1 mm you need high rpmExpect 20,000 rpm or more to get a usable finish on micro bumps.

Measure bumps on the machine before unclampingOnce the vise opens, the part relaxes and the numbers move.

Section 1

What counts as a bump feature

A bump is a raised island left standing on an otherwise cut surface. Typical heights run 0.2–1.5 mm above the floor, with diameters or widths from 0.3 mm to 12 mm. The shape can be round, square, elongated, or a cross. They show up as alignment pins in fixtures, contact pads on busbars, standoffs on covers, and texture features on grips.

The reason bumps are hard is not the height. It is the ratio of height to tool diameter. A 0.5 mm tall pad cut with a Ø6 mm end mill is routine. The same pad cut with a Ø0.8 mm end mill, because the pads sit 1.2 mm apart, is a different job. The tool is now the weakest link in the setup.

Bumps usually fall into three families. Functional bumps carry load or locate a mating part and need tight height control. Contact bumps carry current or heat and care about flatness and surface finish. Cosmetic bumps are texture and only need to look consistent. Each family pulls the process in a different direction.

The first question to answer before programming is whether the bump can be cut from the top at all. If the bump sits inside a pocket deeper than about 3× its own diameter, the tool holder will hit the wall before the cutter reaches the floor. In that case the feature should be redesigned, or cut from a different direction in a second setup.

1
Height to diameter ratio drives everythingAbove 3:1, expect to slow down and step over less.
2
Spacing sets the tool diameterGap between bumps minus 0.2 mm is your maximum cutter size.
3
Function decides the toleranceLocating bumps need height control; texture bumps do not.

Section 2

Tool selection for machine bumps CNC work

For bumps wider than 3 mm, a standard 3-flute carbide end mill in the Ø4–6 mm range is the right call. Aluminum grades 6061 and 7075 run well at 12,000–18,000 rpm with 1,200–2,500 mm/min feed. Three flutes give chip room without the chatter you get from a four-flute tool in a narrow slot.

Between 1 mm and 3 mm, move to a 2-flute or 3-flute micro end mill with a necked shank. The neck is the trick: it lets the cutting portion reach into a pocket while the shank above stays stiff. A necked Ø2 mm tool with a 6 mm neck can reach 8 mm deep where a full-diameter Ø2 mm tool would snap.

Below Ø1 mm, tool life falls off fast and runout becomes the limiting factor. Hold tools in a shrink-fit or high-precision collet chuck rated under 3 μm runout. If your spindle tops out at 10,000 rpm, a Ø0.5 mm tool simply cannot reach the surface speed it needs, and you should plan for a secondary operation instead.

Tool material matters less than coating. An AlTiN or AlCrN coating helps on stainless and tool steel. For aluminum, an uncoated polished tool or a DLC coating prevents built-up edge, which is the number one cause of a torn bump face. Avoid coatings that add thickness on micro tools; a 2 μm coating on a Ø0.4 mm cutter is a measurable change in diameter.

1
> Ø3 mm3-flute carbide, 12,000–18,000 rpm in aluminum.
2
Ø1–3 mmNecked micro end mill, under 3 μm runout.
3
< Ø1 mmShrink-fit holder, 20,000 rpm or higher, or redesign.

Section 3

Programming bumps without chatter

The single most useful programming move is to machine the floor and the bump tops in the same finishing pass. Rough the whole area and leave 0.1–0.2 mm of stock on both the floor and the bump top. Then run one finishing toolpath at full depth that cuts the floor down and leaves the bumps standing. This removes the mismatch you get when the floor and bumps are cut at different times.

Keep the stepover for the finishing pass at 5–8% of the tool diameter when the bump face is a sealing or contact surface. For cosmetic bumps, 10–15% is enough. Radial engagement above 20% on a small tool will push the cutter sideways and leave a taper on the bump wall.

Use climb milling on the finishing pass. Conventional milling on a thin bump wall pulls the tool into the material and produces a wavy edge that shows up under a profile projector. Climb milling also gives a better floor finish, which matters if the floor is a sealing face.

Corner rounding on the toolpath is worth the extra code. A sharp internal corner where the bump meets the floor needs a radius equal to the tool radius. If the CAD model has a sharp corner, either specify a corner radius of at least 0.2 mm or accept that the tool will leave a small radius anyway. Tell the designer which one you chose.

Lead-in and lead-out moves should be tangential arcs, not straight plunges. A straight plunge into the floor next to a bump leaves a witness mark. On a Ø1 mm tool, a 0.5 mm radius tangential entry costs almost no cycle time and removes the mark entirely.

1
Finish floor and bumps togetherOne pass, one Z reference, no mismatch.
2
Stepover 5–8% for functional faces10–15% is fine for texture bumps.
3
Climb mill the finishing passBetter wall quality and floor finish.

Section 4

Workholding and material notes

Bump features are usually small and sit in the middle of a larger part, so the part itself is often the stiffest thing in the setup. That is good news. The weak points are the vise jaws and the tool. Use soft jaws machined to the part profile rather than a standard vise, especially on thin plates where clamping force distorts the floor.

On thin plates under 3 mm thick, the clamping force alone can bow the part by 0.05 mm or more. Machine a support pocket into the soft jaw so the plate sits flat, and keep clamping pressure low. If the plate is very thin, consider bonding it to a fixture plate with cyanoacrylate and cutting the bumps in one pass.

Material choice changes the parameters more than most people expect. Aluminum 6061 cuts cleanly and holds a bump edge well. Stainless 304 work-hardens, so never let the tool rub; keep the feed per tooth above 0.01 mm. Titanium Ti-6Al-4V needs lower surface speed and generous coolant. Plastics like POM and PEEK cut easily but burr at the bump edge, so use a sharp uncoated tool and a light finishing pass.

Coolant strategy matters on micro tools. Flood coolant can deflect a Ø0.5 mm cutter through hydraulic force. Use an air blast or a fine mist instead. On deep pockets, use through-spindle air if available so the chips clear without pushing the tool sideways.

For parts that will be anodized or plated after machining, add 0.02–0.05 mm to the bump height to allow for coating build-up. Hardcoat anodizing can add 0.05 mm per surface, which is enough to close a 0.1 mm gap on a locating bump.

1
Soft jaws over standard viseProfile-machined jaws hold thin parts flat.
2
Air blast on micro toolsFlood coolant bends small cutters.
3
Add stock for coatingHardcoat can add 0.05 mm per surface.

Workflow

Step-by-step bump machining process

Run these in order. Skipping the in-process check at step 5 is the most common cause of a scrapped batch.

1
1. Review the feature against the toolCheck bump width, spacing and depth in the CAD model. The gap between bumps minus 0.2 mm sets the maximum tool diameter. If the required tool is under Ø0.8 mm, flag the feature for DFM review before quoting.
2
2. Confirm the datum and Z referencePick the floor as the Z zero, not the top of the stock. Measure actual stock thickness and enter the true value. A 0.1 mm error in stock thickness becomes a 0.1 mm error in bump height.
3
3. Rough the field, leave 0.1–0.2 mmUse a larger tool for bulk removal. Keep 0.1–0.2 mm on both the floor and the bump top. Do not rough the bump walls to final size; the finishing pass handles them.
4
4. Set the finishing tool and measure runoutLoad the finishing tool and check runout at the cutting edge with a dial indicator. Anything over 3 μm will show as a height variation across the part. Correct in the holder before cutting.
5
5. Cut one test bump and measure itRun a single bump toolpath at reduced feed, then measure height and width on the machine with a touch probe or a height gauge. Adjust the Z offset by the measured error before running the rest of the part.
6
6. Run the finishing pass with climb millingStepover 5–8% of tool diameter for functional faces, 10–15% for cosmetic ones. Tangential lead-in and lead-out. Keep feed per tooth at or above 0.01 mm on stainless.
7
7. Inspect before unclampingMeasure bump height, spacing and floor flatness while the part is still in the vise. Record the values. If a bump is out of tolerance, you can still recut it at this point.
8
8. Deburr and finishRemove the fine burr at the bump edge with a hand lap or a light tumble. If the part will be anodized, leave the extra stock you added in step 1.

Selection guide

Bump size versus process choice

Pick the row that matches your smallest bump. The right column tells you when to walk away from a single-setup approach.

Bump width	Tool diameter	Typical stepover	When it does not work
Over 3 mm	Ø4–6 mm, 3-flute	10–15% of Ø	Pocket deeper than 4× the tool diameter
1–3 mm	Ø1–3 mm, necked	8–12% of Ø	Wall thinner than 0.3 mm
0.5–1 mm	Ø0.8–1 mm, shrink-fit	5–8% of Ø	Spindle below 20,000 rpm
Under 0.5 mm	Redesign or EDM	Not applicable	Almost always; use a second setup
Bump height over 2 mm	Same tool as width	Same as width	Height-to-diameter ratio above 3:1
Soft plastics	Sharp uncoated tool	10–15% of Ø	Bump edge will burr without a light pass

Send the drawing before you commit to a process

Bump features live or die on the tool that can reach them. Send the drawing and we will confirm the smallest bump, the tool diameter and the setup count within 12 hours, with no minimum order quantity.

Get Instant Quote Talk to an Engineer

FAQs

Questions engineers ask about bumps

What is the smallest bump you can machine?

On a milled part, a Ø0.5 mm bump at 0.3 mm tall is practical when the spindle reaches 20,000 rpm and the tool holder holds under 3 μm runout. Below that size, tool life drops and the process becomes unreliable.

For bumps smaller than Ø0.5 mm, the honest answer is usually a redesign or a different process. We will tell you that during DFM review rather than quote a feature we cannot hold.

How do you stop the tool from bending when cutting small bumps?

Shorten the stick-out. Deflection rises with the cube of the length, so cutting 3 mm off the gauge length can reduce bending by more than half. Use a necked tool so the cutting portion is short but the reach is long.

Then control runout. A tool with 10 μm runout behaves like a tool twice its diameter in terms of load. Check runout at the cutting edge, not the shank, and fix it in the holder before cutting.

Can bumps be machined on both metal and plastic parts?

Yes. Aluminum, stainless, steel, titanium, copper alloys, POM, PEEK, ABS and PC all machine into bumps. The parameters change, not the method.

Plastics need a sharp uncoated tool and a light finishing pass to avoid a burr at the bump edge. Stainless needs a feed per tooth above 0.01 mm so the tool does not rub and work-harden.

What finishing options work on machined bumps?

Anodizing, electroless nickel, zinc and silver plating, powder coating and black oxide all work. Bead blasting and tumbling will round the bump edge slightly, so account for that if the bump is a locating feature.

If a bump is a contact pad, choose a conductive anodizing type or mask the pad. Laser marking needs a minimum character height of 1.5 mm, so do not plan to mark on a small bump.

How do you inspect bump height and spacing?

Height is best measured on the machine with a touch probe before unclamping, because the part relaxes when the vise opens. Spacing and width go under a vision system or profile projector.

We inspect 100% of parts before shipment and can supply inspection reports on request. Raw material checks, in-process monitoring and final inspection are all part of the standard route.

When should a bump feature be redesigned instead of machined?

Redesign when the gap between bumps is under 1 mm and the pocket is deeper than 3 mm, when the bump wall is thinner than 0.3 mm, or when the required tool is below Ø0.5 mm. In those cases the cost per part climbs faster than the value the feature adds.

A small corner radius, a wider spacing, or splitting the feature into two operations often fixes the problem without changing the function.