Most drawings call out a finished bore size, tolerance, and finish without saying how to make it. Whether we hone a bore, ID grind it, or do both comes down to six things on the print. These are the bore’s size and remaining stock, its form tolerances, its relationship to other features, the material and heat-treat condition, how a tool can reach it, and the surface finish it needs.
How honing and ID grinding differ
A hone is a rotating tool with expanding abrasive stones that strokes in and out of the bore. The tool or the part floats, so the hone follows the bore’s existing axis. It corrects size, roundness, straightness, taper, and finish, but it will not move the bore or change its angle. Honing is a finishing step that comes after drilling, boring, or reaming, as Sunnen’s honing education material describes.
ID grinding uses a small, high-speed wheel on a quill. The part is held in a chuck or fixture, so the bore is located from the machine and from the surfaces the part is clamped on. That lets us control where the bore sits relative to the rest of the part. When we grind a bore and its related OD or face in one chucking, those features stay concentric and square to each other because the part never moves.
If your print cares about where the bore is, grinding is in the picture. If it only cares about the bore itself, honing usually is the better finish.
Size tolerance and stock removal
Both processes hold tight diameter tolerances, so a tight size callout alone does not decide anything. Honing is the standard answer for bore tolerances of ±0.0002 in. or tighter combined with a fine finish, which Modern Machine Shop covers in more detail.
What decides it is how much material is left. ID grinding removes thousandths of an inch efficiently. Honing removes tenths. Honing can take off more than that, but it is slow and wears stones. When a hardened bore comes in with a lot of stock after heat treat, or it moved during heat treat, we grind it first.
Roundness, cylindricity, and long bores
Honing is the better process for form. It corrects taper, bellmouth, barrel shape, waviness, out-of-round, chatter, and boring marks. The stones contact a long section of the bore at once and average out high spots on every stroke, so the longer the bore, the bigger honing’s advantage.
ID grinding gets harder as the bore gets deeper. The quill has to reach the bottom of the bore, and a long, thin quill bends under grinding load. That bending shows up as taper and size variation along the bore. Steel quills start to struggle past roughly 4:1 or 5:1 length to diameter, which Okuma’s guidance on ID grinding quills explains. Carbide quills extend that, but not indefinitely.
A long, small-diameter bore with a tight cylindricity or straightness callout gets honed.
Position, runout, and perpendicularity callouts
Look at the GD&T. If the bore has a position tolerance, runout or concentricity to an OD, or perpendicularity to a face, the bore is tied to another feature.
Honing cannot fix any of those. If a bore is off location, honing gives you a round, straight, on-size bore in the wrong place. Location has to be set before honing by boring or grinding. If a buyer sends a bore for honing that is already out of position, we will tell them before we touch it.
When the bore has to run true to an OD or be square to a shoulder, we grind it, ideally with the related surfaces in the same setup. Re-chucking a part between operations adds runout every time.
Two or more bores on a common axis, such as in-line or tandem bores, can be brought into alignment with each other by honing them with one long tool that spans both. That aligns the bores to each other. It does not locate them to an outside datum.
Material hardness and heat damage
Hardened parts do not automatically need grinding. We hone hardened steel all the time. Hardness changes the abrasive we pick and how long the cycle takes, not whether honing works.
Heat matters more than hardness. Grinding puts a lot of energy into a small contact area, and in hardened steel too much heat causes over-tempering, tensile residual stress, and rehardening burn. That damage is usually invisible without testing such as nital etch, a point Cutting Tool Engineering explains well. Honing runs cool and is far less likely to distort the bore.
Good grinding practice controls burn. Even so, on thin-walled, heat-sensitive, or fatigue-critical bores, we prefer honing as the final operation.
Blind bores, shoulders, cross holes, and small diameters
Blind bores can be honed, but they need a relief. A relief is a short undercut at the bottom of the bore that lets the stones run past the end of the finished surface. Without one, the blind end stays tight and tapered and takes extra time to correct. If your design can tolerate a relief groove, put it on the print. It is the single easiest change a designer can make to improve a honed blind bore.
ID grinding handles short blind bores and shoulders well, and it can finish the bore and the face next to it in one setup. Depth and diameter are its limits, because the wheel and quill have to fit inside the bore and stay stiff enough to cut accurately.
Honing reaches smaller holes than grinding does. Honing tooling goes down to about .060 in., which is well below where ID grinding gets practical.
Cross holes, ports, keyways, and grooves inside a bore do not rule out honing. They call for keyway-style tooling with wider stones that bridge the gaps. Show every interruption on the print so we can plan the tooling before quoting.
Crosshatch, plateau, and Ra finishes
An Ra limit tells us how smooth the bore has to be. It does not tell us what texture the bore needs, and texture is often the deciding factor.
Honing leaves a crosshatch pattern, and we set the angle with spindle speed and stroke speed. The valleys in that pattern hold oil, which matters in any bore that runs against rings, seals, or pistons. Engine cylinders, liners, and hydraulic bores should be honed. Plateau honing goes a step further by knocking down the peaks and keeping the valleys, which helps rings seat quickly in cylinder liners.
ID grinding leaves a finish with no crosshatch. That is fine for a press-fit bearing bore or a bushing seat, where size, roundness, and runout matter and oil retention does not.
If the bore needs a specific texture, put the crosshatch angle, plateau requirement, or Rz or Rk values on the print. If it only needs to be smooth, an Ra limit is enough.
Honing vs. ID grinding by print requirement
| Requirement on the print | Honing | ID grinding |
|---|---|---|
| Tight roundness, cylindricity, or straightness over a long bore | Best choice | Harder as length to diameter increases |
| Position, concentricity, runout, or perpendicularity to other features | Cannot correct | Best choice, ideally in one setup |
| Large stock removal after heat treat | Slow | Best choice |
| Heat-sensitive, thin-walled, or fatigue-critical part | Best choice | Possible with careful burn control |
| Crosshatch or plateau finish for rings, seals, or pistons | Best choice | Not possible |
| Bore and adjacent face finished together | Not possible | Best choice |
| Very small or deep bore | Best choice | Limited by quill stiffness |
| Blind bore | Works well with a relief at the bottom | Works if short and accessible |
Grinding first, then honing
A lot of the bores we see need both. Grinding sets the bore’s location and its relationship to the OD or a face, and removes most of the stock. Honing then corrects form and brings the bore to final size and texture with very little heat. The hone follows the axis the grinder set, so nothing the grinder established gets lost.
Some parts go the other way. We hone the bore for size and finish, then grind the related face square to it. The order depends on which features are datums on the drawing.
What to send with your RFQ
Send the full drawing, not only the bore detail. GD&T on other features often decides the process.
List the material, hardness, and heat-treat sequence. Tell us whether the part arrives soft or hardened, and whether plating, coating, or nitriding happens before or after the bore is finished.
Tell us how the bore will arrive, including the incoming size, how much stock is left, and how it was made. Send inspection data from the previous operation if you have it.
Note whether the bore is through or blind, whether there is a relief at the bottom, and any cross holes, ports, keyways, or grooves.
Give the finish requirement and tell us what the bore does. A bore that runs against a seal or ring needs a different finish from a press-fit seat.
If the bore has to fit a specific pin, spool, piston, or bearing, tell us. Some bores are sized to the mating part instead of a print dimension.
Include the quantity and schedule, and whether this is a prototype, a repair, or a production run.
List any required inspection method, inspection report, material certification, or first-article requirement.
If something on the print will be hard to make, such as a deep blind bore with no relief, call us before the design is released. Adding an undercut or opening up a callout that does not affect function can lower the cost of every part you buy.
Talk to us about your bore
JTR Specialties has done honing, lapping, grinding, and testing in South El Monte, California, since 1995. We hone, ID grind, and lap in-house, in soft and hardened materials, for aerospace, automotive, and medical customers. Every bore is checked on air gauging before it ships.
Send your drawing and the details above, and we will tell you whether the bore should be honed, ground, or both. Call (626) 444-1124 or email jtrspecialties [at] gmail [dot] com.