My straight (flat) inlay piece is too tight or too loose in its pocket. What allowance should I use?

Why it happens

The Inlay Toolpath already rounds the outside corners of the male part to match the radius the bit leaves in the pocket corners, so the shapes match. What it does not do on its own is leave clearance. With zero allowance both parts are cut to the same nominal size, and any bit wear, machine flex or wood swelling turns that into a fit you have to hammer.

Two rules from the official documentation come first:

• Cut both halves with the same tool. On a pocket with a larger clearance tool, the smaller finishing tool is the one that must match the male tool.
• Allowance is normally applied to the female side, so the male part keeps the true vector shape. On the pocket or hole it is the Pocket Allowance field, and a value there makes the opening larger. On the male side the field is Allowance Offset, and a value there makes the insert smaller.

The fix

1. Measure the real cutting diameter of the bit with calipers and correct it with Edit in the toolpath if it differs from the database value.
2. Cut the male part first with no allowance.
3. Calculate the Female Pocket (or Hole) with a starting Pocket Allowance. The official documentation says 0.01 inch (0.25 mm) or 0.02 inch (0.5 mm) is usually enough when no finish goes on before assembly. A published CNC inlay guide describes tighter targets: 0.002 to 0.005 inch for a press fit that needs a mallet, 0.005 to 0.010 inch for a glue fit, and visible gaps beyond 0.015 inch. The two sources disagree, so treat the official figure as the outer limit and start small.
4. Test on scrap of the same two species. If it is tight, raise the Pocket Allowance a little, recalculate and rerun only the pocket while the board is still clamped.
5. Record the winning value for that bit and wood pair.

Pro tips

• Paint, varnish or stain applied before assembly adds thickness. Allow for it, as the official documentation notes.
• If corners bind but the straights are loose, check that both toolpaths really used the same diameter tool.
• For gaps on a V inlay instead, see the entry on the V inlay depth recipe.