CNC Design Rule Checker

A blind hole cannot be threaded to its floor.

Why: The tap has a lead (chamfered) section that cuts no full thread, and the chips have to go somewhere. Both need space beyond the last full thread.

Instead: Specify the thread depth you need and let the hole be deeper. A drawing that calls full thread to the bottom either deepens the hole or gets less thread than it asked for.

mill or turn

A drilled hole does not land exactly where the drawing says.

Why: The drill follows the surface it starts on and its own deflection, so a drilled hole wanders by an amount that depends on the spot, the material and the depth.

Instead: If the position matters, the position tolerance has to allow for the wander, or the hole has to be spot-drilled, bored or reamed to hold it. Both are operations with a cost, and both are cheaper than discovering it at inspection.

mill or turn

A deep hole of small diameter needs a way for the chip to leave.

Why: The chip is the same volume as the hole. Once the hole is deep relative to its diameter, the chip packs and the drill rubs instead of cutting - heat, wear and a hole that goes off line.

Instead: Expect peck drilling with retracts, or a gundrilling operation on the deep ones. If the drawing allows a larger diameter or a shorter depth, that is the cheap version of the same feature.

mill or turn

An unsupported thin wall bends away from the cutter and springs back afterwards.

Why: The cutting force is a real force, and a thin section has little stiffness against it. The wall measures correctly on the machine under load and incorrectly on the bench.

Instead: Support the wall (a sacrificial web, a filler, a second operation), take light finishing passes, or relax the tolerance on the wall to what the process can actually hold. This is the case where the tolerance, not the geometry, is usually the thing to change.

mill or turn

A tolerance cannot be tighter than the process that makes it. Standard machining holds ±0.005 mm and grinding reaches below it.

Why: Past a point the limit is not the machine but the material, the temperature and the measurement itself. Tightening the number on the drawing does not tighten the process, it only changes what has to be measured.

Instead: Put the tight band on the features that need it - a bore, a mating face, a datum - and leave the general tolerance on everything else. A drawing with one tight tolerance is cheaper than the same drawing with the tolerance moved to the title block.

any process

Where you put the datums decides what the shop has to hold.

Why: Every dimension is measured from a datum, and the datum has to exist as a real, accessible, machined surface. A datum on a raw casting face means the whole part is measured from a surface nobody controls.

Instead: Datum on machined faces, pick the sequence in the order the part is made, and keep them accessible to a probe or an indicator at inspection.

any process

Every machined edge leaves a burr, and a burr is a decision nobody made.

Why: The material has to go somewhere as the tool exits. On a sealing face or a sliding fit a burr is a functional defect; on a painted bracket it is not.

Instead: Say what happens to the edges. A blanket note to deburr everything is not a specification: name the edges that must be free of burrs and the size of the break, and let the rest be.

mill or turn

Engraved or marked text is a cut, with a cutter and a depth.

Why: Engraving is milling with a small tool at a shallow depth. The character height sets the cutter, the cutter sets the feed, and fine detail in the font is what breaks it.

Instead: Give the character height and the depth, use a simple font, and put the marking somewhere the cutter can reach and the material can take it. Marking on a curved or thin surface is a separate operation.

mill or turn