The Price Is Set in CAD, Not at the Shop
Founders negotiate machining quotes as if the number were a matter of opinion. It rarely is. By the time a model reaches a shop, roughly 70 to 80 percent of its cost is locked into the geometry, and the quoting engineer is mostly reporting what your CAD decisions imply about machine time.
Shift the effort upstream instead. The same functional part, redesigned around the machinist's constraints, commonly comes back at half the price with identical performance. That is not haggling, it is a specific form of design for manufacturing, and it takes an afternoon.
Understand What You Are Paying For
A machining quote is roughly: programming and setup, plus spindle time, plus material, plus tooling wear, plus inspection and finishing, plus margin. At prototype quantities the fixed costs dominate. Shop rates in the US typically run $75 to $150 per hour for a 3-axis mill and $120 to $250 for 5-axis, and programming and fixturing for a moderately complex part is often two to four hours before a single chip is cut. The full breakdown is in CNC machining cost.
Two consequences follow. At quantity one, changes that reduce setups matter more than ones that reduce cycle time. And the second unit is far cheaper than the first, so ordering three when you might need two is usually right.
Geometry: The Rules Worth the Most Money
Internal corner radii. An end mill is round, so a square internal corner is impossible. Every internal corner has a radius equal to the cutter, and specifying a small radius forces a small cutter, which forces slow feeds and many passes. Use the largest radius the function allows, and at minimum one third of the pocket depth. Going from a 0.06 in corner radius to 0.25 in on a deep pocket can cut cycle time by half.
Pocket depth relative to tool diameter. Keep depth under 3 to 4 times the cutter diameter. Beyond that the tool deflects and chatters, so the shop drops to light passes or a long-reach tool at extra cost. A pocket 1.5 in deep and 0.25 in wide costs far more than the same volume made wider and shallower.
Wall thickness. Thin walls vibrate. Below about 0.03 in (0.8 mm) in aluminum or 0.02 in (0.5 mm) in steel, the shop has to slow down, add support, or scrap parts. Tall thin ribs are the same problem in the other axis.
Standard hole sizes. A hole that matches a standard drill is one plunge. A non-standard diameter has to be interpolated with an end mill, which takes several times longer. Use fractional, letter, or metric drill sizes, and use standard thread sizes so a tap exists.
Hole depth. Keep drilled depth under 4 times diameter where possible; deeper requires peck cycles and specialty drills, and tapped engagement past 3 times thread diameter adds nothing but cost.
Avoid undercuts and internal features that need special tooling. Internal square corners at the bottom of a pocket, internal keyways, or a groove no standard cutter reaches push the part toward broaching or EDM machining, which is capable and slow and priced accordingly.
Skip engraved text. Engraving a logo with a small tool adds ten to thirty minutes per part; laser marking afterward costs a few dollars.
Setups: Every Extra Orientation Costs Real Money
A setup is one clamping of the part in one orientation. Each new setup means re-fixturing, re-probing, and a fresh chance to accumulate error between features cut in different orientations. On a 3-axis mill each additional setup typically adds $75 to $200 at prototype quantities and loosens the tolerance between features on opposite faces.
Design to minimize them. Put every feature you can on one or two faces, and accept a slightly heavier part if it leaves the fifth face bare. Where features on all sides are unavoidable, ask whether 5-axis is cheaper overall despite the higher hourly rate, since one setup there often beats four on 3-axis; the tradeoff is worked through in 3-axis vs 5-axis CNC machining. Also give the shop something to hold: a flat, parallel pair of faces or extra stock for a soft-jaw grip is worth more than the material it costs.
A related question worth asking honestly: does this need to be one part at all? Splitting a hard single part into two simple plates that bolt together frequently costs less in total, even including hardware and assembly, and it is a standard move in value engineering.
Tolerance and Finish: Pay Only Where It Matters
Standard machining tolerance is around plus or minus 0.005 in and comes free with normal practice. Tightening to plus or minus 0.001 in requires slower finishing passes, in-process measurement, and a higher scrap rate, so expect 30 to 50 percent added cost on the features involved.
Tighten only what mates with something: bearing bores, sealing surfaces, dowel pin locations, press fits. Leave the rest in the general tolerance block. Surface finish behaves the same way, with as-machined 125 microinch Ra as the default and a mirror finish a separate polishing operation. Where the requirement is really about form rather than size, saying so with GD&T often widens the manufacturing window instead of narrowing it.
Material and Stock Size
Machinability varies enormously and shows up directly in the bill. Aluminum 6061 is the reference point at roughly three to four times faster to cut than 304 stainless, with 7075 slightly slower than 6061 and stronger, brass faster still, and titanium and hardened tool steels several times slower with heavy tool wear. Unless the part needs the strength or corrosion resistance, 6061 is the cheap default; the strength and cost comparison is in aluminum vs steel.
Then size the part to the stock. Plate and bar come in standard thicknesses, and a part 0.90 in thick cut from 1.00 in plate leaves both faces to machine, while designing it at 0.98 in lets the shop skim only what it must. Likewise, do not require a 6 in cube of billet to produce a 1 in bracket: material cost and roughing time both scale with what has to be removed.
Design With the Quote in View
Two habits close the loop. Send the model to a shop for DFM feedback before finalizing, since most comment for free on a part they expect to quote, and one email regularly saves hundreds of dollars. And check the quantity assumption: at a few thousand parts a year, the honest answer may be that the part should be cast, molded, or formed, and machining is only the prototype step.
Getting a Part Redesigned for Price
Projects House reviews and redesigns client parts for machining cost: corner and pocket geometry, setup reduction, tolerance rationalization, and stock selection, with a before-and-after quote comparison so the saving is measured rather than claimed. Send your CAD and current quote through our contact form.