Trochoidal Milling and Chip Thinning in Tool Steel

Conventional roughing of tool steel uses a wide radial cut and a shallow depth. Only the bottom few millimetres of the cutter do the work, they do it under high load and heat, and the tool is worn out while most of its flute length is still new. Trochoidal milling, also sold as dynamic or high-efficiency milling, turns this around: a small radial cut, the full flute length, and a tool path that keeps the engagement constant. This article explains how it works, how to correct the feed for chip thinning, and where to start in tool steel.

The idea

In a full slot, the cutter is engaged over 180°. Each tooth spends half of every revolution in the cut, heat builds up, and the chip has nowhere to go. In a trochoidal path, the cutter is smaller than the slot and moves in a series of overlapping loops. It cuts along a thin arc on the forward side of each loop and returns through the open space behind.

The same principle is applied to pockets and open shoulders by CAM software: the path is shaped so the radial engagement never exceeds a set value, even in corners.

Chip thinning

With a small radial engagement, each tooth enters and leaves the material before it reaches the widest part of its arc. The thickest part of the chip is therefore thinner than the programmed feed per tooth.

• Maximum chip thickness = fz × 2 × √(r × (1 − r)), where r = ae ÷ D (valid for r below 0.5)

To keep the chip at the thickness the cutting edge needs, the feed per tooth must be multiplied by the inverse of that factor.

If the feed is not corrected, the chip becomes so thin that the edge rubs instead of cutting. The symptoms are heat, a glazed surface, squealing and rapid flank wear, which is the opposite of what the strategy promises.

Because each tooth is in contact for only a short arc, the cutting speed can usually be raised as well, often by 30–100 % compared with slotting values for the same material.

Starting parameters for tool steel

For coated solid-carbide end mills with five or more flutes, 10–12 mm diameter. "Target chip thickness" is the value after correction for chip thinning.

Start at the lower end, listen to the cut and look at the chips, then increase the feed before the speed.

Worked example

Roughing a pocket in pre-hardened mold steel at 35 HRC with a 10 mm, five-flute end mill.

For comparison, conventional roughing with the same tool at ae = 5 mm, ap = 5 mm, 110 m/min and 0.05 mm per tooth gives a table feed of about 700 mm/min with four flutes and a removal rate of about 18 cm³/min, with all the wear on the bottom 5 mm of the tool.

Two cautions about the comparison. In a closed slot, part of every loop is a return move in air, so the average removal rate is roughly half the cutting value. And the benefit depends on the machine reaching the programmed feed in short, curved moves.

What the method needs

Slots

Slots deeper than twice their width, which are difficult by conventional slotting, are where trochoidal milling shows the largest gain in tool life.

Checking the cut