Custom Machined Parts: 7 Drawing Callouts That Raise Your Quote

When a quote for custom machined parts comes back higher than expected, the geometry usually isn’t the problem. The drawing is. A few callouts, often inherited from an old template or added out of caution, push a simple part into slower machining, extra setups, special tools, and longer inspection. Each one can be justified when the function needs it. Most of the time it doesn’t.

Here are seven callouts we see drive cost on machined parts, and what to put on the drawing instead.

1. A tight title-block tolerance applied to every dimension

A title block that says ±0.001″ on all three-place decimals applies that tolerance to every feature on the part, including the ones that only need to clear a bolt. Standard CNC machining holds about ±0.005″ (±0.125 mm) without special effort. Tightening to the ±0.001″ to ±0.002″ range typically costs 1.5 to 2 times as much, and going to ±0.0004″ or tighter can cost four times as much or more, often with a grinding step added.

Instead: set the general tolerance to what most features need, and call out tight tolerances only on the features that mate, seal, or locate. Our post on what ±0.001″ actually means for your program covers the inspection side of this.

2. Sharp internal corners

An end mill is round, so it leaves a radius in every internal vertical corner. A drawing that shows a sharp inside corner forces EDM, broaching, or a very small cutter running slowly. A good rule is an internal corner radius of at least one third of the pocket depth, with the same radius on every internal edge so one tool can finish them all. A 0.5″ deep pocket wants a radius of about 0.17″ or larger.

Instead: dimension the radius the part can accept, or add a dog-bone relief if a square mating part has to drop in. Our fillet vs. chamfer guide covers edge treatments.

3. Deep, narrow pockets

Cutting tools perform best at a depth of two to three times their diameter. Past that, they deflect, chatter, and need slower feeds. Pockets deeper than about four times their width get expensive fast.

Instead: open up narrow pockets, reduce depth where the function allows, or split the part into two pieces that bolt or bond together.

4. Long threads and non-standard holes

Thread engagement past about three times the hole diameter adds little holding strength but adds tapping time and broken-tap risk. Blind threaded holes need unthreaded relief at the bottom, about half the hole diameter. Hole depths beyond four times the diameter need special drills, and odd diameters that don’t match standard drills force interpolation with an end mill.

Instead: limit thread depth to what the fastener needs, use standard drill and tap sizes, and give blind holes room at the bottom.

5. GD&T that doesn’t match function

Geometric dimensioning and tolerancing is the right tool for controlling how features relate. Problems start when every surface gets a profile callout, or when the datum scheme doesn’t reflect how the part actually mounts. The shop then has to fixture and inspect to datums that don’t match assembly, and you may pay for CMM time on features nobody checks in service.

Instead: choose datums based on how the part locates in the assembly, and apply tight geometric controls only to functional features.

6. Surface finish tighter than the part needs

An as-machined finish is typically around 125 µin Ra (3.2 µm). A blanket callout of 32 Ra or finer on every surface adds finishing passes, polishing, or grinding. Cosmetic requirements written as “no visible tool marks” with no defined inspection standard cause disputes at receiving.

Instead: call out finer finishes only on sealing, bearing, or sliding surfaces, and define cosmetic requirements with a reference sample or a clear standard. If the part is anodized or plated, remember the coating adds thickness. Our finishing team can tell you which features to mask.

7. Thin walls and tall, slender features

Thin walls vibrate under the cutter and make tolerances hard to hold. As a starting point, keep metal walls above about 0.03″ (0.8 mm) and plastic walls above about 0.06″ (1.5 mm). Tall features with a height-to-width ratio past about 4:1 have the same problem. Raised (embossed) text adds machining time too; engraved text in a simple sans serif font is faster.

Instead: thicken walls where you can, add ribs for stiffness, and engrave text rather than embossing it.

A quick pre-quote checklist

• Is the general tolerance set to what most features need?
• Do internal corners have a radius a standard tool can cut?
• Are pocket depths and hole depths within about four times width or diameter?
• Are threads, holes, and tap drills standard sizes?
• Do datums match how the part mounts?
• Are fine finishes called out only where the function needs them?
• Are walls thick enough to machine without chatter?

How PE reviews drawings for cost

Every drawing PE receives gets engineering review before it goes to a shop. When a callout is driving cost without a clear functional reason, we flag it and ask before we quote. You decide whether to change it. Our CNC machining network handles everything from simple brackets to tight-tolerance defense and aerospace components, and every part is inspected in San Clemente before it ships.