2.7 Plan a Pocket-Milling Operation

Key Takeaways

  • Check that the selected cutter can reach the requested cavity and inside corners. A tool radius larger than the inside corner radius cannot produce that corner by simple profile milling.

  • A drilled entry, linear ramp or helical ramp requires different cutter capabilities and free space. Match the entry to the tool data and actual setup.

  • Roughing leaves controlled stock for finishing. Distinguish side allowance from floor allowance.

  • For the illustrated internal circular path, centerline radius equals pocket radius minus effective cutter radius. Check whether the controller or CAM has already adjusted the path and feed.

Last updated: November 2026

2.7 Plan a Pocket-Milling Operation

The NIMS crosswalk includes pocket milling. A pocket is a cavity with a floor or a material boundary that constrains where the cutter can enter and travel. A closed pocket is surrounded by material at the entry level. An open-sided pocket can permit a side entry in free space. Inspect the print and fixture together before choosing how to open, rough and finish the cavity.

Check Cutter and Entry Fit

A print calls for a 10-mm-deep closed pocket with a 4-mm inside corner radius. A 10-mm end mill has a 5-mm radius and cannot reproduce that 4-mm corner with simple 2D profile milling. A 6-mm end mill has a 3-mm radius, leaving a 1-mm centerline radius at the finished corner in ideal geometry. A shop could rough the broad area with a larger cutter and finish the residual stock with the smaller tool. Verify the remaining material and cutting engagement where the tool enters that corner. A very small tool or a long unsupported extension can deflect. Check flute reach, holder access, the narrowest part of the cavity, and the machine’s available Z travel.

Entry optionWhen it can workCheck before cutting
Enter from outsideAn open side provides a clear approachClamp and holder clearance through the whole approach
Enter through a prepared holeA drilled opening gives room for the cutterHole diameter and depth accommodate the complete entry path
Linear rampThe cutter supports ramping and the pocket has enough lengthMaximum ramp angle and required travel
Helical rampThe cutter supports circular ramping and there is room for the orbitDiameter range, ramp pitch, floor clearance and chip removal

The selected tool’s data govern allowable ramp angles and entry conditions. Some cutters are designed for side engagement or partial ramps. A tool that can follow a flat finishing path is not necessarily suitable for plunging in the center of solid stock.

Plan Depths and Allowances

Use cutting passes appropriate to the cutter, material and workholding. Keep stepover, the lateral spacing between passes, separate from stepdown, the axial change between levels. Plan a way to evacuate chips. Recut chips can damage the finish or tool, especially when they collect deep in the cavity.

Suppose the floor is at work Z−10.000 mm and the process plan calls for 0.200 mm of floor stock before finishing. The lowest roughing pass is at Z−9.800 mm. A 0.300-mm side allowance means the roughing edge stops 0.300 mm inside each nominal wall. For two opposing straight walls this reduces the roughed opening by 0.600 mm along that width. A later wall pass and floor pass can use different strategies. Verify both dimensions on the first part.

The Haas G150 general pocket cycle is one controller-specific way to process a closed boundary. Haas uses a subprogram for the geometry and an X or Y roughing increment. Its K finish amount pertains to the pocket wall. The depth sequence is a separate check. This distinction also applies when a CAM program uses separate wall and floor allowances.

Worked Circular Pocket Trace

Consider finishing an existing circular opening to 24 mm with an 8-mm effective cutter diameter. If programming the tool center directly, its orbit radius is (24−8)/2=8(24-8)/2=8 mm. The cutter’s outer edge reaches 8+4=128+4=12 mm from the pocket center. If the nominal edge already describes a part-boundary path and full cutter compensation is expected, do not also program this reduced centerline radius.

The center and cutting edge travel different distances in one orbit. For this ideal circular geometry, assume the tool guidance gives a target wall-path advance of 360 mm/min and the control expects a tool-center feed. The centerline path diameter is 16 mm, so the centerline rate is 360×16/24=240360\times16/24=240 mm/min. This is a geometric conversion. Tool engagement, feed modes and any compensation or feed conversion by the software need separate verification. Applying the reduction twice would feed the cutter too slowly for the intended calculation.

Sources: NIMS CNC mill competency crosswalk, Sandvik milling and circular-feed formulas, Sandvik entry strategies, and Haas G150.

Test Your Knowledge

A 2D pocket has a finished inside corner radius of 4 mm. Which cutter could reach that corner by contouring, assuming enough reach and room?

A

12-mm cutter

B

10-mm cutter

C

6-mm cutter

D

16-mm cutter

Test Your Knowledge

Work Z0 is at the top and the pocket floor is Z−10.000 mm. What is the roughing floor if 0.200 mm must remain for finishing?

A

Z−10.200 mm

B

Z−9.800 mm

C

Z−10.000 mm

D

Z+9.800 mm

Test Your Knowledge

What tool-center orbit radius gives a finished 24-mm circular opening with an 8-mm cutter when programming the center directly?

A

8 mm

B

12 mm

C

16 mm

D

4 mm

Sections you finish are checked off in the contents.