The part is designed against a tool that has a shape
A milling cutter is not a point. It has a diameter, a length, a flute geometry and a holder behind it, and every one of those dimensions constrains what the machine can produce. A CAD model is indifferent to this; a machine shop is not. The gap between the two is where manufacturability problems come from.
Thinking about the cutter while designing removes most of that gap. Two questions cover a surprising amount of ground: how deep is the feature relative to its narrowest width, and can a tool of that size physically get to it without the holder colliding with the part?
Depth-to-diameter is the number that decides price
A cutter cutting a slot or pocket has to reach the bottom, and reaching deep with a small tool means a long, slender cutter that deflects under load. Deflection shows up as taper, chatter and a surface finish that has to be corrected, and correcting it costs a second operation.
A useful working rule is to keep pocket depth to about four times the cutter diameter and no more than roughly three times the internal corner radius. Beyond that, the shop is choosing between a slow, light cut with a long tool and an EDM operation - both of which are legitimate, and both of which are more expensive than a shallower pocket would have been.
Internal corners are cutter radii, not sharp corners
A vertical internal corner produced by milling has the radius of the cutter that made it. Asking for a sharp internal corner is not asking for precision; it is asking for a process change, because the only common way to produce one is EDM.
The cheapest drawing is one with corner radii that are generous and standard, so a common cutter can be used. Where a sharp corner is genuinely needed - a locating feature, a seal, a keyway - say so, and let the shop quote the EDM operation deliberately rather than discovering it.
Undercuts, dovetails and side features
A feature that is wider at the bottom than at the opening cannot be reached from above. Machining it requires either a second setup from another direction or a special cutter, and both change the cost and the positional accuracy of the part.
The way to design around it is to ask whether the function really needs the undercut, or whether it can be reached by flipping the part. A T-slot cut from the side is straightforward on a machine with the right fixture; the same slot specified on a face the machine cannot index to is a redesign waiting to happen.
Thin walls and tall features want support
Thin sections deflect under cutting force. A wall a few tenths of a millimetre thick will move away from the cutter and spring back, and the finished thickness will not be what the drawing says. The same is true of tall, narrow bosses.
The design answers are to add thickness where it does not hurt, to leave material that can be removed in a later operation once the part is more rigid, and to avoid long unsupported sections. Where a genuinely thin wall is required, that is a fact worth flagging on the drawing so it can be planned rather than discovered.
Holes, and the depth a drill can manage
A drilled hole has its own depth-to-diameter limit, and it is tighter than a milled pocket. Beyond roughly four times diameter, chip evacuation becomes the problem and the drill wanders; beyond about eight, the operation needs peck drilling or a gun drill, and it becomes a specialist job.
Hole entries and exits matter too. A drill breaking out of a curved or angled surface wanders unless it is started flat, and a hole that exits into another feature can leave a burr in a place nobody can reach to remove. Both are visible in the model before the part is cut.
References
The dimensional rules that govern how a feature is specified - datums, feature control frames and the difference between a general and a specific tolerance - are set out in geometric dimensioning and tolerancing and formalised in ASME Y14.5. The cost behaviour of tightening those callouts follows the published convention for engineering tolerance.
Frequently asked
How deep can a pocket be milled?
A common working limit is about four times the cutter diameter, and a depth that also respects the corner radius - roughly three times the radius. Inside those limits a standard cutter does the job. Beyond them the shop is choosing between a slow light cut with a long tool and an EDM operation, and either costs more.
Can I specify a sharp internal corner?
You can, but it is a process change rather than a tolerance. Milling leaves the cutter's radius in the corner. A genuinely sharp internal corner is produced by EDM, which is a legitimate requirement where the function needs it - a keyway or a locating feature - and worth flagging early so it is quoted deliberately.
How thin can a machined wall be?
It depends on the material, the wall height and the cutter, but thin walls deflect under cutting force and will not hold the dimension on the drawing. Adding thickness where it costs nothing, and removing material after the part is rigid, is usually cheaper than fighting the deflection.