The machining questions shops actually ask — answered.

Start from surface speed (SFM) for your material and convert to spindle RPM, then set the feed rate from chip load:

RPM = (SFM × 3.82) ÷ tool diameter. Feed rate (in/min) = RPM × chip load per tooth × number of flutes. Metal removal rate (in³/min) = width of cut × depth of cut × feed rate.

The SFM comes from the material (aluminum is high, Inconel is low), and the chip load per tooth scales with tool diameter. RobbJack's Speeds & Feeds calculator does all of this from 67 years of tested data — pick a tool or a material and diameter and it returns roughing and finishing numbers.

Chip load per tooth (CLPT) is how much material each flute removes per revolution — it's what actually controls tool life and finish. Too light rubs and work-hardens the cut; too heavy overloads the edge.

As a rule of thumb, chip load scales with tool diameter. RobbJack's data uses a material factor times the diameter — for example a 1/4" tool runs about .004" per tooth in aluminum and far less in tough alloys. Use the calculator for an exact starting point, then tune to your chip color and sound.

Climb milling for most applications — RobbJack recommends it whenever your machine has good backlash control. Climb milling engages the flute at full chip thickness tapering to zero, which gives better finishes, lower cutting forces, and longer tool life.

Conventional milling can work-harden some ferrous materials (stainless, high-temp alloys) and tends to leave a rougher finish. The main reason to avoid climb is excessive backlash on an older manual machine.

Aluminum is RPM-limited, not surface-speed-limited — in practice you run the maximum RPM your spindle allows and set the feed from chip load. RobbJack's aluminum charts literally say "use Max RPM" across all diameters.

Starting chip loads run roughly .004" per tooth at 1/4", .008" at 1/2", and .016" at 1". Run a 2- or 3-flute polished tool, climb mill, and take an axial depth deeper than the corner radius to keep the cut quiet. RobbJack high-velocity tools have run aluminum at 450 IPM with no chatter.

Titanium runs at low surface speed and is grade-sensitive: commercially-pure titanium around 350 SFM, 6Al-4V around 230 SFM, and 6Al-6V around 180 SFM. Chip load per tooth is roughly tool diameter × .0048 for CP and 6Al-4V.

Keep the tool in the cut (titanium hates dwelling and rubbing), climb mill, use plenty of coolant, and reach for a variable-helix tool to control heat and chatter. RobbJack's high-efficiency finishers have cut titanium at up to 75 IPM.

Inconel and nickel super alloys are the slowest common materials — start around 100 SFM with a chip load near tool diameter × .0036. The heat goes into the tool, so a tough substrate, an AlTiN coating, and a rigid setup matter more than speed.

For aggressive roughing, RobbJack's SPS Super Python has delivered up to a 1000% metal-removal-rate increase in Inconel 718 versus standard tooling. Keep feeds steady, never let the tool dwell, and use high-pressure coolant where you can.

Trochoidal (or peel) milling takes a light radial cut at a high axial depth along a circular tool path, so the tool engages a small arc at a time. It spreads heat and wear over the full flute length and lets you run high feeds in tough materials without overloading the edge.

Use it for slots and pockets in stainless, titanium, and high-temp alloys, especially with multi-flute finishers. RobbJack's calculator includes a trochoidal mode that raises the allowable chip load when you select it.

Your CAM almost certainly already has it, just under its own name — it's all high-efficiency milling (HEM): Mastercam Dynamic Milling, Fusion 360 Adaptive Clearing, Esprit Profit Milling, VoluMill, and Surfware TrueMill. As a starting point, size the tool to about 50% of the slot width, take 1.5–2× diameter axially, and set radial width to 3–10% for difficult alloys or 25–50% for easier non-ferrous.

Usually you want the shortest tool that reaches the cut — but aluminum with a Mirror Edge tool breaks that rule. Up to about 4:1 length-to-diameter in aluminum, do all the machining with one Mirror Edge tool: it stays chatter-free so you don't have to slow down, which avoids the slow cycle times long tools normally force.

Beyond 4:1, or in tougher materials, rough with a short tool to remove most of the material, then step up to a longer tool only where you need the reach. Using a single long tool for everything actually costs cycle time, because you have to back off speeds and feeds for the stickout.

Use a tool about 50% of the slot width (or the tightest area you're cutting), take an axial depth of 1.5–2× the tool diameter, and set the radial width by material: 3–10% of diameter for difficult alloys like titanium and nickel, and 25–50% for easy non-ferrous materials.

The radial width controls how long the edge is in the cut, which controls heat: at 100% width the tool is engaged 180° and is cutting half the time; at 50% width that drops to 90° and 25% of the time; at 25% width, 60° and 17%; at 10% width, just 37° and 10%. Lighter radial engagement spreads heat and wear over the whole flute, which is why a light-radial, full-depth trochoidal pass runs so much harder than a slot. RobbJack's calculator has a trochoidal mode that raises the allowable chip load to match.

Use a 2- or 3-flute polished solid-carbide end mill made for non-ferrous work. RobbJack's AL3 (3-flute, 35° helix, mirror-polished edge with chip breakers on longer lengths) is the workhorse; the 2-flute A1-201 reduces required horsepower for full slots, and the 3-flute A1-303 reduces chatter.

For maximum removal on rigid, high-HP/high-RPM machines, step up to the FM/FMHV high-velocity lines. For gummy or soft aluminum and plastics, single-flute PM routers prevent material from sticking and melting in the cut.

Reach for a variable-helix multi-flute carbide tool with an AlTiN coating. RobbJack's XG (4- and 5-flute variable helix) roughs and finishes; the 6- and 8-flute XF (45° helix) is the high-efficiency finisher; and the honed-edge Super Tuffy (ST/STR) handles tougher work.

These have run 304 stainless at 400 SFM and 24 IPM with up to a 500% increase in removal rate. Note that free-machining 303 stainless runs far faster than 304/316. Climb mill and keep the setup rigid.

Use a tough-grade variable-helix tool with AlTiN, run at low surface speed with steady feed. RobbJack's NS (4-flute variable helix) is a proven choice — it was developed cutting 6Al-4V titanium flap tracks for aircraft wings — and the XG/XF families handle stainless through Inconel.

For the most aggressive roughing in these materials, the SPS Super Python is the curated flagship, rated for stainless, super alloys, Inconel, titanium, and steel to 40 HRc.

Use AlTiN-coated die/mold geometry matched to the cut: a 2-flute ball (RobbJack DM) for 3-D cavities and cores, a toroid corner-radius tool (TM) for helical bores and tight corners, and a 4- to 10-flute high-helix tool (HM) for open floors and walls.

RobbJack rates these for 40, 50, and 64 HRc, and the AlTiN coating is good in material up to 70 HRc. Reduce depth of cut as hardness rises, use air or mist coolant above 40 HRc, and enter by helical interpolation or from off the part.

Graphite is abrasive and best cut dry with a diamond-coated solid-carbide tool. RobbJack's P38 Lightning and P820 diamond-coated end mills are built for graphite — the P38 uses a thinner diamond coating for a sharper edge and lower cost.

Diamond coating gives roughly 10–20× the life of uncoated carbide in graphite. Speed bands by grade: soft graphite 1000–2000 SFM, medium 750–1500, hard 500–1250. Run good dust extraction.

Use a PCD (polycrystalline diamond) or diamond-coated tool — carbon fiber destroys uncoated carbide. RobbJack's CPCD-203 PCD-tipped router is built for trimming composites: its 118° drill point plunges without back-side blowout and it leaves no delamination, uncut fibers, or fiber pull-out, with over 13,000 linear inches of life in aircraft CFRP.

Compression routers (CR/CE) give a clean edge on both faces, and diamond-coated drills handle hole-making. PCD runs 10–30× the life of carbide on abrasive composites.

Match flute count to material and operation. Fewer flutes give more chip room; more flutes give a better finish and faster feed when chips are small.

Aluminum and non-ferrous: 2 or 3 flutes for chip clearance. Steel, stainless, and high-temp alloys: 4 flutes for general work, 5 flutes for roughing-plus-finishing, and 6–8 flutes for high-efficiency finishing and trochoidal paths. For roughing in gummy or soft material, fewer flutes evacuate chips better.

Soft, foldable intraocular-lens materials are harder to cut cleanly than the old rigid plastics, so they need specialized small-diameter geometry — polished cutting edges and very sharp geometry that shears the material instead of tearing it.

RobbJack produces these geometries down to roughly 250 microns (.010") in diameter. The same approach — polished, sharp, micro-diameter tools held to tight tolerances — applies to other delicate medical and micro-machining work.

Both beat uncoated carbide on abrasive composites; the choice comes down to plastic content, geometry, and diameter. PCD (polycrystalline diamond) has ground edges that start and stay sharper than diamond-coated, gives the longest life, and can be resharpened — it's the go-to for higher-plastic-content materials and for trimming CFRP (RobbJack's CPCD router runs over 13,000 linear inches in aircraft CFRP).

Diamond-coated carbide wins where you want more flutes or finer geometry, in lower-plastic-content composites, and at the small diameters PCD tips can't reach — you grind any geometry on the carbide blank and then grow diamond on it. Rule of thumb: PCD for the sharpest edge and longest life in higher-plastic material; diamond-coated for geometry flexibility, lower-plastic material, and small tools.

Stacks — composite over aluminum or titanium, or honeycomb-cored panels — are tough because each layer wants a different geometry, and the transitions cause delamination and burrs. Use a tool that enters and exits cleanly: a compression router pushes the top and bottom plies inward for a clean edge on both faces, and a PCD or diamond-coated tool survives the abrasive plies.

Control the feed through layer transitions and back the part where you can to prevent push-out on the exit side.

It depends on the composite and your dust/handling setup. Many carbon-fiber and graphite jobs run dry with good extraction, because coolant can contaminate the laminate and create a slurry — and diamond/PCD tooling handles the heat.

Where heat or fiber pull-out is a problem, light coolant or air assist helps clear chips and keep the edge cool. Match it to the material and whether the finished part can tolerate coolant.

Match the drill to how many holes you need and the material's plastic content. For a few holes or manual work, solid carbide is fine but wears fast; for production, use diamond-coated or PCD.

Diamond-coated carbide gives 10–20× the life of solid carbide and lets you grind specialized points: an 8-facet tip with a double angle reams out delamination, a traditional 4-facet single angle covers most composites, and an elliptical "bullet" point spreads the cut over a larger area to kill delamination and uncut fibers. PCD drills hold an even sharper edge for higher-plastic-content material and can be resharpened. Keep the setup rigid and the spindle RPM steady — both drive consistent hole quality.

It scales with material thickness, but a 1/4" PCD drill typically gets about 3,000–8,000 holes in roughly 1/4"-thick CFRP, depending on how sensitive the part is. Dedicated small-diameter perforation tools go much further — RobbJack has run up to 40,000 holes in carbon fiber and 80,000 in fiberglass with a single tool on aircraft acoustic panels.

The keys to high, predictable hole counts are diamond-coating adhesion, a spindle that actually holds RPM (watch for speeders that drop RPM under load), and careful, non-contact tool handling.

Overlooking rigidity. When the part vibrates, tool life drops and the process becomes unpredictable — so the more rigid the workpiece and fixture, the longer the tool lasts and the faster and more repeatably you can run.

The best fixture is a vacuum fixture matched closely to the part. When that's not practical, low-cost fixes work: sandbags to damp un-rigid areas, or strapping and taping down unsupported corners on a family-of-parts fixture. Treat composite machining as a whole process — tool selection, programming, fixturing, and tool holders together — and most of the pain disappears.

Match the family to your reach and your machine. A1-201 (2-flute) is for heavy stub roughing and reducing horsepower on full slots; A1-303 (3-flute, polished, Mirror Edge) is the general workhorse up to about 3:1 length-to-diameter and targets machines under 25K RPM.

For longer reach, AL3 adds 3–5×D cutting length, thru-coolant, corner radii, and chip breakers, and finishes deep walls in a single pass. FM is the necked Mirror Edge tool with a Feather Blend transition for deep pockets and thin walls over 3:1, and FMHV is a balanced 3-flute built for ultra-high-RPM, high-horsepower machines. All but the A1-201 carry Mirror Edge to run chatter-free at max RPM (with coolant).

Match the coating to the material's main challenge — heat, abrasion, or built-up edge:

• AlTiN (Scorpion Stinger): best for hardened steel over 50 HRc, titanium, Inconel/super alloys, and stainless; ideal for high-speed and dry machining.
• TiCN (Python Scales): titanium and nickel alloys, abrasive materials, interrupted cuts, and cast iron.
• TiN (King Cobra): general purpose for soft and unalloyed steels, forming tools, and injection molds.
• DLC (Black Mamba): aluminum, copper, high-silicon aluminum, graphite, and composites — it prevents built-up edge and runs dry.

Use DLC (diamond-like carbon) or a polished uncoated tool — not AlTiN, TiCN, or TiN. Those titanium-based coatings are designed for ferrous heat and actually cause aluminum to stick and build up on the edge.

RobbJack's Black Mamba DLC is extremely lubricious (coefficient of friction around 0.05–0.15), so aluminum, copper, and high-silicon aluminum shear cleanly instead of welding to the flute. It's also the coating that lets you cut aluminum dry or with minimal coolant.

Yes — use AlTiN. When cutting hardened steel, AlTiN forms an aluminum-oxide layer at the cutting edge that acts as a heat shield, blocking heat from the carbide and pushing it into the chip instead.

That's why RobbJack uses AlTiN on its die/mold and hardened-steel lines, and it's effective in material up to 70 HRc. Do not use TiN on steel above 50 HRc. Above 40 HRc, run air or mist coolant and reduce your depth of cut.

Yes, with the right tool. A DLC-coated or polished uncoated carbide end mill can cut aluminum dry or with minimal-quantity lubrication because the slick, low-friction surface keeps aluminum from welding to the edge.

RobbJack's Black Mamba DLC is the coating to choose when coolant or MQL isn't available. Coolant still helps with chip evacuation and finish, but DLC is what makes dry aluminum cutting practical.

Yes. RobbJack owns and operates its own ISO-9000 PVD coating facility in Lincoln, California, and will coat or re-coat any brand of tool — not just RobbJack's. Running coating in-house means no shipping it out to a third party and faster turnaround.

You can pick from the four coatings (AlTiN, TiCN, TiN, DLC) to match your material. Note that once a tool is coated or otherwise modified, it's non-returnable.

Yes. Our in-house PVD and DLC coating facility coats more than cutting tools — we coat many medical parts and components, because the strict handling and quality procedures required for coating carbide tools are very similar to what delicate medical parts need.

If you have parts or instruments that would benefit from a hard, low-friction, or wear-resistant coating, we can run them.

Use a 6% cobalt carbide with about a 1-micron grain — not a submicron grain. Most cutting-tool makers stock only a 10% micrograin carbide, which doesn't take a reliable diamond coating, so you can't just send any carbide tool out to be diamond-coated.

The reason is in the process: to grow diamond, the cobalt is leached from the surface first — otherwise a graphite layer forms and the coating wipes right off — and the 6% / ~1-micron grade leaches and coats cleanly. RobbJack and Crystallume publish which grades work, so ask if you're unsure.

RobbJack builds its tools on three tungsten-carbide grades, each a different point on the hardness–toughness curve:

C2 — 6% cobalt, 1 µm fine grain: the hardest and most wear-resistant of the three. Tuffy — 10% cobalt, 0.8 µm submicron grain: the balanced all-rounder. Super Tuffy — 15–16% cobalt, 0.8 µm submicron grain: the toughest and most shock-resistant.

The grade isn't one-size-fits-all — RobbJack matches the substrate to each tool line's job, the same way it matches geometry and coating, so every tool starts from the carbide that gives the highest performance for its application.

Cobalt content — the binder that holds the tungsten-carbide grains together. More cobalt buys toughness; less cobalt buys hardness and wear resistance.

C2 (6% cobalt, 1 µm fine grain) holds the keenest edge the longest — best where abrasion, not shock, is the limiting factor. Tuffy (10% cobalt, 0.8 µm submicron) adds binder for toughness while the finer grain keeps strength and edge quality high — a versatile middle. Super Tuffy (15–16% cobalt, 0.8 µm submicron) carries the highest binder content to resist chipping and shock loads — built for interrupted cuts and demanding, unforgiving conditions.

Tungsten carbide isn't a single material — it's extremely hard carbide grains held in a cobalt binder, and the ratio sets the tool's personality. Lower the cobalt and the tool gets harder and more wear-resistant but more brittle; raise it and the tool gets tougher and more chip-resistant but wears faster.

That's why one "carbide" tool can shatter in an interrupted cut while another dulls early in an abrasive one — they were the wrong points on the curve for the job. RobbJack picks the point per tool line: 6% cobalt (C2) where wear dominates, 10% (Tuffy) for balance, and 15–16% (Super Tuffy) where the cut hammers the edge.

Finer carbide grains sharpen the edge and raise strength at any given cobalt level — a 0.8 µm submicron structure can be ground to a keener, more consistent cutting edge that resists micro-chipping better than coarser material.

RobbJack's Tuffy and Super Tuffy grades are both submicron (0.8 µm), which is how Super Tuffy can carry 15–16% cobalt for shock resistance without giving up edge quality, and why Tuffy performs above its 10% binder class. The fine-grain C2 (1 µm) trades a slightly coarser structure for the lowest binder content and maximum wear resistance.

By the failure mode the application will impose. If the edge will die by abrasion — high-silicon aluminum, composites, long production runs in free-cutting material — wear resistance wins and the harder, lower-binder C2 is the right substrate. If the edge will die by chipping — interrupted cuts, scale, flex, tough alloys that hammer the flutes — shock resistance wins and Super Tuffy's high binder content protects it. Tuffy covers the wide middle where both matter, which is why it's the grade under lines like the SPS Super Python rougher and RobbJack's die/mold toroids.

You don't have to pick the grade yourself — it's engineered into each tool line along with the geometry and coating. Pick the tool for your material and operation (the Tool Finder or an application engineer will get you there) and the right carbide comes with it.

Chatter is vibration feeding on itself — break the harmonic and stiffen the system. The fastest fixes: use a variable-helix tool (offset flutes that damp the resonance), shorten the tool or add a neck to increase rigidity, and grip the shank tightly (shrink-fit or Weldon flats).

RobbJack's patented Mirror Edge geometry is purpose-built to damp vibration and eliminate chatter on thin walls, deep pockets, and tools over 3:1 length-to-diameter (use coolant with it). On necked aluminum tools, take an axial depth of cut deeper than the corner radius — that alone quiets many cuts.

Premature chipping usually means the edge is too sharp for the material, the cut is too light (rubbing instead of cutting), or there's vibration. A honed edge fixes the first: RobbJack's T-Process strengthens the edge to eliminate chipping in steel, stainless, and super alloys.

Also confirm you're climb milling, running enough chip load to cut rather than rub, using the right coating (AlTiN for heat, DLC for aluminum), and holding the tool rigidly. Don't add a honed edge for aluminum or plastics — those want a sharp edge.

Take a light finishing pass with a high-flute-count tool, climb mill, and let the geometry do the work. For floors, RobbJack's Wiper Flats clean up swirl marks (skip them on thin floors, since they add contact). For necked tools, the Feather Blend transition reduces staircase marks, stress risers, and plunge swirl lines.

A 6- or 8-flute finisher, the right chip load, and a rigid holder make the biggest difference. For ball-end tools, reduce feed about 10% on the finishing pass.

Pull-out comes from heavy axial loads overcoming the holder's grip. The best fix is a tighter grip: RobbJack's anti-pull-out shank — an h4 shank tolerance, the tightest in the industry — adds up to 150% more gripping force, and it holds even in extreme cuts (there are tools taking full slots in aluminum at over 200 horsepower without coming out of the spindle).

Also match the holder to the job: use a shrink-fit or equivalent, or order the tool with Weldon flats (-FL) so a set screw locks it. If you're running through-spindle coolant and can't drill the tool, coolant grooves are a lower-cost alternative to through-the-tool holes.

Don't reach for a long flute length — use a necked tool. A neck (reduced-diameter section behind a short cutting length) is far more rigid than a long-length-of-cut tool, so it deflects less and lasts longer, while clearing the walls of a deep pocket.

RobbJack can add a neck and reach to most standard tools in 1–2 days, and offers ER solid extensions and Accuhold holders held to under .0002" runout for long-reach work. Keep the cutting length just long enough for the job.

Use Mirror Edge whenever chatter is a risk — deep pockets where the tool sticks out more than 3:1 length-to-diameter, or thin walls — where it produces a finish far superior to a chattering cut. The one time to skip it: if the application isn't prone to chatter, a standard (non-Mirror-Edge) edge leaves a slightly better finish.

The deciding factor is simple — if you have chatter, Mirror Edge helps. Note that Mirror Edge tools must be run with coolant.

Often, yes — it depends on the material and the cut. Two levers help most: programming to control the angle of engagement (which limits heat build-up), and an in-house PVD coating that acts as a heat shield on the tool.

Steels and many heat-treated alloys cut dry well. But gummy materials, and ones that don't carry heat out in the chip — nickel alloys, titanium, even aluminum — cut much better with flood coolant. If you need to get away from flood, cold-air guns and newer cryogenic options (CO₂, liquid nitrogen) can help.

We'd strongly recommend against it — we see a lot of tool failures from shop-ground flats. Every diameter has a specific, tight flat dimension (the width is held to under .001") so the set screw locks against the sides of the flat as well as the bottom. Grind it slightly off and the tool can pull out or break.

Because of that, RobbJack grinds Weldon flats (-FL) on our tools at no charge — so you get the flat exactly where and how you need it, from the factory.

Almost always, it's being run like a carbide burr: high RPM, slow feed, and light multiple passes. That's a grinding action — it builds heat, melts the resin, and abrades the diamond. The fix is counter-intuitive: lower the RPM and raise the feed so the sharp diamond edge shears the material in one full-depth pass.

For full-slot trimming, run about 800–1,000 SFM — roughly 8,150–10,000 RPM on a 3/8" tool, about 6,100 RPM on a 1/2" tool — at a high feed (around 80 IPM on a 3/8"), with depth of cut up to about 2× diameter, cut to net shape. Shearing instead of grinding keeps the tool cool and dramatically extends life.

The mistake most people make is skim-passing the wall — light finish passes on a tall, thin wall that just let it flex and push away from the cutter. Don't. Instead, waterfall down and finish at every Z-depth: rough and finish each depth of cut to final size before you step deeper, and once a wall is thin at a given depth, never cut it at that depth again.

Leave at least .100" of stock on the wall for the finish pass — not a light skim. Because you finish at every level, the wall being cut is only ever as tall as your step-down, so it stays rigid. Example: a 1/2" tool cutting .200" deep is finishing a wall that's .100"+ wide and only .200" tall at the cut — short and stiff, so it can't push away. A 2"-tall thin wall machined this way behaves like a .200"-deep part.

For the tool, get maximum rigidity: the shortest length of cut that reaches, minimum wall contact, and neck it for reach (a neck is far more rigid than a long flute). Climb mill, run a Mirror Edge tool with coolant, and use sharp, polished flutes — not a honed edge. RobbJack's FM and FMHV families are built for thin walls and deep pockets over 3:1.

Thin floors have very little thermal mass, so heat from the cut distorts them and the floor can start oil-canning — and a standard end-mill face rubs at the center where surface speed drops to zero. The fix is geometry built for it.

RobbJack's thin-floor geometry reduces oil-canning, residual stress, and heat build-up, keeps the aluminum's heat treatment intact, and eliminates the rubbing and zero-surface-speed problem. It can be added to any tool — ask application engineering to spec it on the tool you're using.

Any thickness from 0.0020" to 0.2500" is standard — you order in ten-thousandths of an inch, and RobbJack grinds it. Thickness is held to +.0002"/−.0000", diameter to +.002"/−.000", and the arbor ID is held tight to assure arbor fit and reduce runout.

Most thicknesses from .008" to .250" ship within 48 hours. Saws thinner than .010" are specials and non-returnable.

Match pitch to material: coarse pitch (10° rake, fewer teeth) for non-ferrous metals, and fine pitch (5° rake, roughly double the teeth) for ferrous metals. The coarse tooth gives chip room in soft, gummy materials; the fine tooth supports the edge and improves finish in steel and stainless.

Fewer teeth in contact also means more chip load per tooth, so a coarse saw clears chips and cuts cooler in aluminum, while a fine saw leaves a cleaner edge in steel.

It depends on the saw thickness. As a rule, when depth of cut exceeds about 3× the saw thickness you should add a hub or double the standard concavity for clearance; when it exceeds about 5× the thickness, step up to a K-Series saw (double concavity, alternate-tooth chamfer, and flat/parallel hubs) so the saw doesn't bind.

RobbJack's saw calculator applies these rules automatically and recommends the K-series when the cut is deep relative to thickness.

A thru-coolant arbor delivers coolant directly to both faces of the slitting saw and clamps it far more securely than a standard arbor. RobbJack's NAB ultra-precision arbors grip the saw up to 15× more tightly — so it can't slip or spin on the arbor — which keeps it running true, flushes chips out of the slot, and dramatically reduces saw failures.

They come in 1/4" to 1-1/4" bores with published torque specs and carbide spacers, and pair with CF carbide thru-coolant flanges. Coolant to the cut is the single biggest improvement for deep or gummy slitting. (Note: this is the arbor's grip on the saw — separate from the up-to-150% anti-pull-out grip a holder has on a tool shank.)

Start with a thoroughly clean saw, arbor, and tool holder, all in excellent condition, and use only arbors and holders held to .0002" on diameter and runout. "Ring in" the saw so it seats dead flat — clearances can be under .0001" — and hand-tighten with moderate force; don't over-tighten.

Then check runout. Indicating the side of the saw, keep side run-out under .0005". For saws thicker than .020", measure tooth-to-tooth by spinning the saw opposite its cutting direction and noting the highest reading per tooth — the spread should stay around .0001". Set coolant to heavy, equal flow on both faces (unequal coolant causes problems), and listen: a correct cut sounds smooth, with no re-cutting of chips. Start from RobbJack's recommended speeds and feeds.

It's how the saw contacts the arbor and hub. A C-Series saw makes taper contact on its outer ring. A K-Series saw sits flush against the arbor and hub — its hub and tooth thickness are the same — which increases surface contact and gripping force, reduces runout, and improves accuracy. A hub is essential for any gang (stacked) application.

Step up to the K-Series — with its alternate-tooth chamfer, double concavity, and flat parallel hub — anytime the depth of cut is more than 3× the saw thickness; it works so well it solves the large majority of slitting-saw problems by minimizing saw slippage, eliminating chip packing, and reducing torque. Two exceptions: K-Series isn't made under .020" thick, and skip it on full-radius saws or when the corner radius exceeds 10% of the saw thickness. Note that any thickness up to .250" is standard at the same price and delivery as catalog sizes — minimums scale with diameter (.002" on saws up to 1", .004" up to 2", .006" above).

Yes — and it's a standard order, not a special. Any thickness between the thinnest and thickest saw in a series is standard, in .0001" steps. The middle four digits of the part number are the thickness in ten-thousandths of an inch: a .0300"-thick 2" saw with a 1" arbor hole is C20-0300-32-48, even though the catalog lists .0280" and .0312".

The order is priced as the next thicker saw that appears in the catalog, at standard delivery. Minimum thickness depends on diameter: .002" (3/4"–1"), .004" (1¼"–2"), .006" (2¼"–4"); K-Series starts at .020".

Pick the geometry by the feature: a 2-flute ball-end tool (RobbJack DM, 30° helix) for 3-D cavities and cores; a toroid corner-radius tool (TM) for helical bores and tight corners; and a multi-flute high-helix tool (HM, 4–10 flutes, 45°) for open floors and walls.

All three are AlTiN-coated and rated for 40, 50, and 64 HRc. RobbJack's speeds & feeds engine even auto-selects the HM for open areas and the TM for tight cavities.

With the right geometry and AlTiN coating, RobbJack die/mold tools are rated up to 64 HRc, and the AlTiN coating remains effective in material up to 70 HRc. The key is reducing engagement as hardness rises.

Depth of cut scales down with hardness — for example a ball-end tool runs about 10% of diameter axial at 30–40 HRc, 5% at 40–50 HRc, and 4% at 50–60 HRc. Use air or mist coolant above 40 HRc, climb mill, and enter the cut by ramping or helical interpolation.

The SPS Super Python is RobbJack's flagship roughing line — Tuffy-grade carbide with a variable-helix, all-center-cutting geometry built to take the most aggressive cuts in the toughest materials: stainless, super alloys, Inconel, titanium, and steel up to 40 HRc.

It comes in 4- and 5-flute, stub through extra-long lengths, with seven standard corner radii and optional flats for high-torque cuts. The headline result is up to a 1000% increase in metal removal rate in Inconel 718. Its motto: "strikes harder, cuts faster."

Variable helix means the flutes are ground at different (offset) helix angles instead of all the same. That breaks up the regular tooth-impact frequency that causes resonance, so the tool damps its own vibration — the result is chatter-free cuts, better finishes, and longer tool life.

It's the headline geometry on RobbJack's NS, XG/MXG, and XF/MXF lines for steel, stainless, titanium, and high-temp alloys, and on the SPS Super Python. It's especially valuable in tough or interrupted cuts where chatter would otherwise kill the edge.

Yes — RobbJack regrinds and re-coats any brand of tool, not just its own, with in-house PVD coating and what it considers the best delivery in the industry. You can request the same grinds and finishes RobbJack puts on new tools.

If a tool is too far gone, it's returned marked "No Work Done" at no charge, or you can recycle it through RobbJack's GO GREEN carbide-recycling program for a 10% discount certificate toward your next regrind order.

Solid carbide holds a sharper, more wear-resistant edge at much higher temperatures than high-speed steel, so it runs faster, lasts longer, and holds tighter tolerances — which is why it dominates high-performance milling of alloys, hardened steel, and abrasives.

Versus indexable tooling, a solid-carbide end mill gives a true cutting geometry down to small diameters, finer finishes, and the ability to take light, accurate finishing passes. RobbJack grinds its tools to an h4 shank tolerance and holds runout under .0002" so that accuracy reaches the part.

It depends on the tool. PCD-tipped drills and routers are restored by re-lapping the diamond — a real advantage of solid-tip PCD — and solid carbide regrinds normally. Diamond-coated tools are a different story: re-coating means stripping back to carbide and re-growing the diamond in a high-temperature reactor, so in most cases it isn't cost-justified versus a new tool, and most customers don't resharpen them.

As with any regrind, if a tool is too far gone we return it "No Work Done" at no charge, or recycle the carbide through our GO GREEN program for a discount toward your next order.

Every .001" diameter from .005" to .062" is a standard size in the SS (stub) and SR (standard-length) miniature lines — that's 58 standard diameters, not just the common fractions.

If your job needs something in between, RobbJack hand-selects miniatures to ANY diameter to the nearest .0002" under .062". Need a .0376" tool? That's a regular order, not a special. Hand-selecting means we measure and pick tools whose actual ground diameter lands on your target — the way micro-tool work usually demands.

Yes — for flat-bottomed holes, spotting on angled or curved surfaces, and interrupted-cut hole starts. There are two versions: an aluminum/non-ferrous version (uncoated or DLC, ground sharp) and a steel/stainless version with a T-Process honed end for edge strength.

Starting speeds and feeds: aluminum about 1000 SFM at 100 IPM; 1018 steel about 300 SFM at 12.5 IPM; 304 stainless about 50 SFM at 2.9 IPM. Check the catalog for speed and feed adjustments by diameter and depth.