CadVex blog · 18 September 2026

7 DFM checks that change the price of a CNC machined part

Sharp corners, deep pockets, thin walls, tapped holes, extra setups: the DFM issues that change a CNC quote, and what to ask the customer.

By CadVex · 6 min read

Most of a machined part's price comes from the obvious inputs: material, stock, removed volume and setups. Quotes usually go wrong on details: a corner radius, wall thickness or tolerance note that decides whether the part runs with standard tools or ties up a machine with a small, long cutter.

This checklist is for the estimator reviewing an RFQ: why each issue adds cost, how to spot it and what to ask the customer.

Not every DFM finding should move the price. Some add tooling, cycle time or setups and belong in the estimate; others are notes for review or questions for the customer. Telling them apart is most of the job.

1. Sharp internal corners and small corner radii

A rotating cutter always leaves its own radius in an internal vertical corner. Zero-radius pocket corners cannot be milled as drawn.

Why it costs more: a truly sharp corner needs wire or sinker EDM, broaching or a design change. A small radius forces a small end mill: lighter cuts, rest machining after the roughing tool and a higher risk of breaking a tool. In a deep pocket, that small tool must also be long.

How to spot it: check each vertical corner against the cutter you would use at that depth. A common guideline is a radius slightly larger than the cutter radius, and at least about a third of the pocket depth. Floor-to-wall edges are different: a flat end mill leaves them nearly sharp.

What to ask: is the sharp corner functional, for example to clear a square mating part? If so, suggest a corner relief (dogbone) or a larger radius. A corner already drawn with a radius a standard cutter produces is a note, not a cost.

2. Deep pockets and narrow slots

Depth only matters relative to the tool that fits: the narrowest width or smallest corner radius sets the largest usable cutter.

Why it costs more: longer stick-out means deflection and chatter. Depth of cut and feed come down, extra passes keep walls straight, and necked or long-reach tools may be needed.

How to spot it: compare depth with the diameter of the largest cutter that fits. As a starting point, about three to four diameters is often routine; beyond that, expect long-reach tooling and slower cutting. The real limit depends on material, tool, holder and machine, so treat any ratio as a prompt to review, not a rule.

What to ask: does the pocket need its full depth? Lightening pockets often do not. Could it be wider, opened from the other side or given a larger corner radius?

3. Thin walls and thin floors

Thin is relative to height and span. A 1 mm wall 5 mm tall is a different problem from one 40 mm tall.

Why it costs more: thin walls deflect and ring, leaving chatter marks and walls that taper out of tolerance. They need light passes, careful sequencing and sometimes custom fixturing. Thin floors drum and can distort when the part leaves the vise. Scrap risk rises late in the cycle, when most of the value is already in the part.

How to spot it: look for tall walls between pockets, thin ribs and floors under large pockets. Design guides often cite about 0.8 mm for metal walls and 1.5 mm for plastics as starting points, but the height-to-thickness ratio and the wall's tolerance matter as much.

What to ask: can the wall be thicker, shorter or tied to a neighbouring wall with a rib? If not, can its thickness tolerance open up?

4. Holes: small, deep, angled and tapped

Holes look simple, which is why they get underquoted.

Why it costs more: small drills are fragile, and deep holes add peck cycles, through-coolant drills or deep-hole tooling. A drill entering an inclined or curved face walks, so it needs a spot face, another setup or multi-axis positioning. Blind tapped holes need drill depth beyond the thread for the tap lead and chips, and a tap broken late in the cycle can scrap a finished part.

How to spot it: compare depth with diameter on every hole; a common guideline treats about four diameters as routine, with time and risk climbing beyond that. Check entry faces and thread callouts. Thread engagement beyond roughly 1.5 to 2 times the nominal diameter, depending on material, usually adds little holding strength.

What to ask: can the hole go through, or use a standard drill size? Can the thread be shorter, with clearance at the bottom? Can an angled hole be square to a face already being machined?

5. Extra setups, 4/5-axis access and undercuts

Every new orientation is another setup: fixturing, indicating, work offsets, probing, a first-piece check and extra handling on every part.

Why it costs more: setup and programming are fixed costs, so they dominate small batches. Each re-clamp also adds error between features cut in different setups. Compound angles need a 4- or 5-axis machine or angled fixtures. Undercuts such as T-slots, dovetails, internal grooves and back-side chamfers need special cutters or EDM, which add cost and lead time.

How to spot it: count the directions features must be reached from, and check for tight tolerances between features in different setups.

What to ask: can features move to a face already being machined? Is the undercut functional? On your side, check whether one 3+2 setup could replace several 3-axis setups. See also the main cost drivers in a CNC machining quote.

6. Tight tolerances and fine finishes applied everywhere

A tight general tolerance in the title block, or a fine finish on every face, often reflects a template default, not a functional need.

Why it costs more: it means finishing passes, slower feeds, closer control of tool wear and temperature, more in-process measurement and longer inspection. Holes may need reaming or boring; faces may need grinding. Finishes finer than the commonly cited as-machined Ra 3.2 µm typically need extra passes or a secondary process.

How to spot it: a STEP file usually carries no tolerances, so read the drawing: general tolerances, tight callouts on non-functional features, finish symbols on every face.

What to ask: which features are functional? Suggest a general tolerance class such as ISO 2768-m for the rest, and keep tight tolerances and fine finishes for bores, sealing faces and mating surfaces.

7. Sharp edges, deburring and cosmetic requirements

"Break all sharp edges" and "no burrs" are reasonable notes. They still cost time that scales with quantity.

Why it costs more: manual deburring is per-part labour that is easy to underestimate. Burrs inside cross-drilled holes may need special tools or thermal deburring as an outside process. Knife edges, where two faces meet at an acute angle, chip and burr easily. Cosmetic requirements add handling, protective packaging and rejection risk, and anodizing does not hide tool marks.

How to spot it: count edges and cross holes, read the edge and cosmetic notes, and look for chamfers in many sizes.

What to ask: can one chamfer size cover every edge? Can the cosmetic faces be named? Can a knife edge get a small flat?

Price it, ask about it, or note it

Price it when the work is real and the design is unlikely to change. Ask when a small change would remove the cost. Note it when the geometry is already what a standard tool leaves. When you ask, quote both ways so the customer sees what the change is worth.

How CadVex helps with DFM review

CadVex analyzes the STEP geometry and flags manufacturability concerns, such as small internal radii, deep holes or pockets, thin walls and additional setup requirements. Each finding is connected to the geometry: click it and the affected faces are highlighted on the 3D model. Findings explain the likely impact and give practical guidance for review, with issues and notes kept separate.

The estimator still makes the call. You can try it on one of your own parts, in the browser or locally with CadVex Desktop.