Skip to content
Free Ground over $80 · Free Priority over $125⚡ Kinetic Carving members save 17.76% →
High Country Tools

CNC Guide

Upcut vs Downcut vs Compression Bits: Which CNC End Mill to Use

By Caleb G ·

The Short Answer

The three bits differ in one thing: which way the spiral moves the chips. That decides which face of the cut comes out clean.

Side-by-Side Comparison

UpcutDowncutCompression
Chip directionUp and out of the cutDown into the cutUp at the tip, down above it
Top edgeCan fuzz or splinterCleanClean, once the downcut section reaches the top face
Bottom edgeCleanCan splinter on through-cutsClean
Chip clearing and heatBest; runs coolestWeakest; chips pack in deep slotsGood, but it needs full-depth passes
Effect on the partLifts the part; use tabs or good hold-downPresses the part downBalanced
Depth per passDeepest of the threePockets up to about 1.5x the bit diameter, with a strong vacuumFirst pass deeper than the upcut section
Best forDeep pockets, profiles, roughing, thick hardwood, plasticsShallow pockets, signs, inlays, V-carve clearing, veneersCutouts in plywood, melamine and veneered panels
Avoid forVeneered or laminated faces where the top edge showsDeep slots without good dust collectionShallow pockets that never reach the downcut section

Upcut End Mills

An upcut end mill lifts chips up out of the slot like an auger. Because the chips leave the cut, the bit doesn't re-cut them, so it runs cooler and lasts longer. That makes it the right choice for deep pockets, profile cuts through thick hardwood, and roughing passes on 3D carves.

The tradeoff is the top edge. The upward spiral pulls surface fibers up, so plywood veneer and some hardwoods fuzz or splinter along the top of the cut. On a roughing pass that doesn't matter. On a finished visible edge, use a downcut or compression bit instead, or plan a light finishing pass.

Upcut bits also pull up on the part. Small parts can lift or shift at the end of a cutout, so use tabs, an onion-skin final pass, or a good vacuum or screw hold-down.

For plastics and acrylic, use an O-flute upcut. Its single polished flute clears big chips and keeps the plastic from melting.

Downcut End Mills

A downcut end mill pushes the cut down into the material. It leaves a crisp, splinter-free top edge every time, which is why it's the go-to bit for signs, inlay pockets, clearing V-carve pockets, and anything with a veneer or laminate on top. It also presses the part down onto the spoilboard instead of lifting it.

The tradeoff is chip packing. Chips have nowhere to go but down, so in a deep slot they pack in, the bit re-cuts them and heat builds. A quality downcut is my personal choice for pocketing, because it leaves a sharp edge with no splintering.

One caveat: keep downcut pockets to about 1.5x the bit diameter deep (about 3/8" for a 1/4" bit), and run a strong vacuum or dust collector so chips are pulled out before they build heat. For anything deeper, rough with an upcut and finish with the downcut.

On a through-cut, the bottom face of the part can splinter. For through-cuts in two-sided material, that is the job for a compression bit.

Compression End Mills

A compression bit has a short upcut section at the tip and a longer downcut section above it. The two spirals push toward each other, toward the middle of the stock. The upcut tip keeps the bottom face clean, and the downcut section keeps the top face clean. The result is clean edges on both faces of plywood, melamine, veneered panels and cabinet parts.

The first-pass rule

The most common compression mistake is a shallow first pass. If the first pass is shallower than the upcut section, only the upcut tip is cutting, and it fuzzes the top face just like an upcut bit would. Make the first pass deeper than the upcut section, so the downcut flutes reach the top face from the start.

These HCT compression bits have a 0.20" upcut section, so make the first pass at least about 0.23" deep:

BitPart no.Upcut sectionFirst pass at leastPrice
1/4" Compression End Mill1/4" Compression End MillCOM-14-DLC0.20"0.23"$39.00
3/16" Compression, 1/4" Shank3/16" Compression, 1/4" ShankMCO-316-DLC0.20"0.23"$38.00
4mm Compression, 1/4" Shank4mm Compression, 1/4" ShankCOM-4mm-DLC0.20"0.23"$34.00

For the 3/8" and 1/2" compression bits, use the first-pass depth in the HCT tool libraries, which are already set to clear the upcut section.

On lighter machines, the first pass can't always go that deep without overloading the bit. In that case the libraries say ROUGH FIRST: rough most of the depth with an upcut or downcut bit, then make one full-depth finishing pass with the compression bit.

Mortise compression bits

The 1/8" and 3/16" mortise compression bits have a very short upcut section, so the downcut part reaches the top face on a shallow first pass. They're made for shallow pockets, mortises and dados in plywood, where a standard compression bit's upcut section would be longer than the pocket is deep.

Starting Settings From the HCT Tool Libraries

These are the v9.3 library starting points for 1/4" 2-flute bits in 1/2" to 3/4" Baltic birch plywood. Upcut and downcut share the same numbers. The compression bit runs a deeper first pass at a lower feed so the downcut flutes reach the top face.

Machine class (examples)1/4" upcut or downcut (END-UC2 / END-DC2)1/4" compression (COM-14)
Light hobby (Shapeoko 3 & 4, X-Carve, LongMill)70 ipm, 0.081" per pass45 ipm, 0.23" first pass
Rigid hobby (Onefinity, Shapeoko 5 Pro, AltMill)100 ipm, 0.125" per pass91 ipm, 0.25" per pass
Business class (ShopSabre, Avid, CAMaster)250 ipm, 0.175" per pass229 ipm, 0.35" per pass

These are starting points. Adjust by sound and chip size. For other materials, bits and machines, use the free Vectric and Fusion 360 tool libraries or the Feeds & Speeds Calculator.

Which Bit for Which Job

JobBitPart no.Price
Plywood cutouts on a hobby machine1/4" Compression End Mill1/4" Compression End MillCOM-14-DLC$39.00
Cabinet boxes and full sheets of 3/4" ply3/8" Compression End Mill3/8" Compression End MillCOM-38I-DLC$74.00 – $88.00
Production sheet goods on 3 HP+ spindles1/2" 2-Flute Compression End Mill1/2" 2-Flute Compression End MillCOM-12-DLC$89.00 – $99.00
Shallow pockets, mortises and dados in plywood1/8" 2-Flute Mortise Compression1/8" 2-Flute Mortise CompressionMCO-18-DLC$24.00
Deep pockets and profiles in hardwood1/4" 2-Flute Upcut End Mill1/4" 2-Flute Upcut End MillEND-UC2-DLC$34.00
Smooth upcut finishing passes1/4" 2-Flute Upcut Finishing End Mill1/4" 2-Flute Upcut Finishing End MillEND-ULH-DLC$38.00Out of stock
Fast roughing and bulk removalRIPPER 1/4" Roughing End MillRIPPER 1/4" Roughing End MillRIPPER-14-DLC$39.00
Signs, lettering pockets and V-carve clearing1/8" 2-Flute Downcut End Mill1/8" 2-Flute Downcut End MillEND-18D-DLC$22.00 – $29.00
Inlay pockets and fine detail1/16" 2-Flute Downcut End Mill1/16" 2-Flute Downcut End MillEND-116D14-DLC$23.00 – $28.00
Clean-topped pockets in hardwood1/4" 2-Flute Downcut End Mill1/4" 2-Flute Downcut End MillEND-DC2-DLC$34.00
Finer finish on a rigid machine1/4" 4-Flute Downcut End Mill1/4" 4-Flute Downcut End MillEND-DC4-DLC$34.00
Larger clean-topped pockets on bigger machines3/8" 2-Flute Downcut End Mill3/8" 2-Flute Downcut End MillEND-38D2F-DLC$59.00Out of stock
Acrylic and plastics1/4" O-Flute Upcut End Mill1/4" O-Flute Upcut End MillOFS-14U-DLC / OFL-14U-DLC$32.00 – $34.00

If You Only Buy One of Each

All HCT end mills are solid Japanese carbide with rainbow DLC coating. Browse every size: upcut end mills, downcut end mills, compression bits. New to CNC bits? Start with The 5 Must-Have Bits for Your CNC Router.

Upcut vs Downcut vs Compression FAQ

What is the difference between upcut and downcut bits?

An upcut bit pulls chips up and out of the cut, so it clears material fast and runs cooler, but it can splinter the top edge. A downcut bit pushes chips down and leaves a crisp top edge, but it packs chips into the slot, so keep passes shallow and use good dust collection.

When should I use a compression bit instead of an upcut or downcut?

Use a compression bit for through-cuts where both faces show: plywood, melamine, veneered panels and cabinet parts. Its upcut tip keeps the bottom face clean and its downcut section keeps the top face clean. Upcut and downcut bits each leave one face rough on a through-cut.

How deep should the first pass be with a compression bit?

Deeper than the bit's upcut section, so the downcut flutes reach the top face. For the HCT 1/4" compression bit, with a 0.20" upcut section, make the first pass at least about 0.23" deep. On light machines, rough with an upcut or downcut bit first, then finish with one full-depth compression pass.

Which bit is best for cutting plywood on a CNC?

A compression bit, for cutouts. It leaves both faces of the plywood clean in one pass. For pockets in plywood, use a downcut bit, which keeps the top veneer from splintering, or a mortise compression bit for shallow pockets and dados.

Which bit is best for hardwood?

An upcut bit for deep pockets, profiles and roughing, since it clears chips and runs cool. A downcut bit when the top edge has to be crisp, such as signs and inlays. For a clean top edge on a deep cut, rough with an upcut and finish with a downcut.

Why does my upcut bit splinter the top edge?

The upward spiral lifts the surface fibers as it cuts. That's normal for an upcut bit, especially in plywood veneer. Switch to a downcut or compression bit for visible edges, or rough with the upcut and make a light finishing pass with a downcut.

Can I use a downcut bit for deep cuts?

You can, but chips pack into the slot, heat builds and the bit wears faster. Keep downcut pockets to about 1.5x the bit diameter deep, run a strong vacuum, and switch to an upcut or compression bit for deep slots and through-cuts.

What bit should I use for acrylic and plastic?

An O-flute upcut. Its single polished flute clears large chips and keeps the plastic from melting and re-welding behind the cut.

Thanks for reading! Shop CNC bits, grab the free Vectric and Fusion 360 tool libraries, or try the Feeds & Speeds Calculator.