Guide
Helical interpolation for holes and threads: how does it affect roundness, finish and cost?
Helical interpolation is a CNC milling move in which the machine drives the cutter around a circle in X and Y while feeding steadily in Z, so an end mill or thread mill cuts a hole or thread larger than itself. It lets one tool make many hole sizes and is the standard way to mill threads, but the hole’s roundness and size now depend on the machine’s circular accuracy and on tool deflection, not on a fixed-size drill or reamer.
By Saola Manufacturing engineering team · Published · Updated
On this page
What is helical interpolation, and how is it different from drilling or boring?
A drill, reamer or boring bar cuts a hole whose size is set by the tool; a helically interpolated hole is generated by the machine’s path, so its size is set by the program and the cutter compensation. That is the root of both its flexibility and its limits.
Tool maker Sandvik Coromant describes circular ramping, also called helical or spiral interpolation or orbital drilling, as moving in a circle in X and Y while feeding axially in Z at a set pitch, and presents it as an alternative to drilling. It notes that circular ramping is always preferred to linear ramping, because radial engagement is lower, cutting is smoother, pure down-milling is possible and chips evacuate better.
Three axes are enough; the move is a standard circular-plus-linear command on any CNC milling control, not a five-axis operation. The same move with a thread mill, advancing one thread pitch per revolution, produces a thread. Our thread milling vs tapping guide covers when that beats a tap, so this guide stays with plain holes and what the method does to hole quality.
When is helical interpolation the right way to make a hole?
It suits holes larger than a standard drill a shop would keep, holes in castings where the cored hole is undersize or off-center, holes that need a flat bottom, and low-volume parts where buying a special drill or boring setup is not worth it. It is usually slower than drilling a standard size.
On a cast part, a drill follows whatever the cored hole gives it, while an interpolating end mill cuts on a programmed center, so it can pull a hole back onto position. On a blind hole, an end mill fed to the center leaves a flat floor; Sandvik notes that a cutter too large for the hole leaves a center pip that fouls the cutter, while one that is too small leaves a core, so cutter size has to suit the hole. For a range of diameters on one part, one end mill can replace several drills or a boring head set to each size.
The trade-off is time and accuracy. A twist drill makes a hole in one plunge; interpolation takes many revolutions of the path, and for tight-tolerance holes it is usually a roughing or semi-finishing step before a boring bar or reamer brings the hole to size.
| Question | Helical interpolation | Drill (plus ream) | Boring bar |
|---|---|---|---|
| What sets the hole size | Program path and cutter compensation | Tool diameter | Tool setting |
| What sets roundness | Machine circular accuracy, backlash, deflection | Tool and spindle; reamer follows the drilled hole | Spindle; single-point cut |
| Corrects position of a cored or drilled hole | Yes | No, follows the existing hole | Yes |
| Many sizes with one tool | Yes | No | With adjustment |
| Flat-bottom blind hole | Yes, if cutter size suits | No, drill point | Limited |
| Cycle time on a standard-size hole | Slower | Fastest | Medium |
| Typical role on a fit hole | Rough or semi-finish | Finish (ream) | Finish |
How does helical interpolation affect hole roundness and size?
An interpolated hole is only as round as the machine’s circular motion, so backlash, servo mismatch and axis squareness print directly into the hole. Tool deflection adds taper and makes the hole smaller than programmed, especially with long, slender cutters.
Machine builders and service engineers check circular motion with a ballbar. Renishaw describes its ballbar as detecting minute variations in radius as it follows a programmed circular path, revealing geometric, dynamic or play-related errors in the machine, and offers report formats to standards such as ISO 230-4 and ANSI B5.54. The same errors that show on a ballbar plot, such as small steps where an axis reverses direction, show up as flats or bumps on an interpolated bore.
Deflection is the second effect. The cutter bends away from the wall under cutting load, so the hole comes out undersize, and because the load and the tool stick-out vary along the depth, the hole can be tapered. Shops compensate with cutter radius offsets and a light finishing pass. A final full circle at constant depth, without Z feed, removes the helical step left by the ramp. If the hole is a bearing or dowel fit, expect the shop to finish it with a boring bar or reamer rather than rely on interpolation alone.
What surface finish does helical interpolation leave?
A helical toolpath can leave a faint spiral lead mark on the wall and a witness line where the path enters and exits. A finishing pass usually takes care of it, but if the wall is a seal or sliding surface, the drawing should state the surface texture it needs.
Down-milling, which Sandvik notes circular ramping allows, generally leaves a better wall than up-milling. Even so, the wall of an interpolated hole is a milled surface made by the side of the cutter, not a reamed or bored surface, and its texture depends on feed per tooth, stepover, rigidity and the finishing pass. For a static clearance hole that does not matter. For an O-ring bore, a valve seat or a piston bore, write the surface texture on the drawing, and if spiral marks are unacceptable, say “no spiral tool marks” instead of naming a process. Our surface finish symbol guide shows how to write the texture requirement.
Does helical interpolation make a part cheaper or more expensive?
It lowers cost when it replaces special tools, boring setups or tool changes, and raises cost when it replaces a single drill plunge on a standard size. The biggest savings show up on large holes, odd sizes and small lots.
The cost logic is tooling versus cycle time. A family of parts with many hole sizes can run with a few end mills instead of a drill and reamer for every size, which saves tool inventory and changeovers. On high-volume parts with standard holes, the extra path time per hole adds up, and a drill or a dedicated combination tool is usually cheaper. You can influence this from the drawing: standard drill sizes on clearance holes, generous tolerances where the function allows, and tight tolerances only where a fit needs them. The CNC machining cost drivers guide covers the wider picture.
What should the drawing say about holes that may be interpolated?
The drawing should state the hole size, tolerance, form, surface texture and position, not the method. Let the shop decide between drilling, interpolating, boring and reaming, and state any functional requirement that would rule a method out.
- Size and tolerance. A clear tolerance or fit class tells the shop whether interpolation alone is enough.
- Form. If roundness or cylindricity matters, put a number on it; size limits alone allow some lobing and taper.
- Surface texture. State it on seal and sliding bores.
- Bottom form. Say whether a blind hole needs a flat bottom.
- Threads. Call out the thread and class; whether it is tapped or thread milled is the shop’s choice unless the function requires one.
The engineering drawing symbols guide covers how to read and write the hole notes themselves.
How does Saola choose the method for large holes?
The machining method for each hole is chosen at drawing review against the size, tolerance and form on the print. Simultaneous five-axis machining is not offered, which does not limit helical interpolation, since the move needs only three axes.
The CNC milling page describes the work at the lead plant: mostly second-operation machining of castings, including bores bored and reamed to print and tapped holes. On a new part, the first-article inspection report covers every toleranced dimension on the drawing, as described on the quality page. If your part has large or odd-size holes, send the drawing through the quote form, and the review will say how each one is made.
Frequently asked
Is helical interpolation the same as circular interpolation?
Circular interpolation is the move in a circle in two axes. Helical interpolation adds a simultaneous linear move in the third axis, so the tool spirals down instead of cutting a single circle.
Does helical interpolation need a five-axis machine?
No. It uses two axes in a circle and a third axis moving linearly, which any three-axis CNC mill can do.
Can helical interpolation hold an H7 tolerance?
It is usually used to rough or semi-finish such holes, with a boring bar or reamer for the final size. Whether interpolation alone is enough depends on the machine, the tool and the hole, which is why the drawing should state the tolerance and leave the method open.
Why is my interpolated hole smaller at the bottom?
Tool deflection. The cutter bends away from the wall under load, more so at full depth with a long tool. A finishing pass and offset compensation reduce it.
Is thread milling a form of helical interpolation?
Yes. A thread mill follows a helical path advancing one pitch per revolution, which is why one thread mill can cut several diameters with the same pitch.
Sources
- Ramping: two axis linear and circular, Sandvik Coromant, accessed November 2026
- QC20-W ballbar system, Renishaw, accessed November 2026