Cellborne CNC Design Guidelines

Purpose & scope

Design parts to these guidelines and they can be machined at Cellborne quickly, at the quoted price, without a design-for-manufacturing (DFM) back-and-forth. The rules apply to metal and plastic parts machined on Cellborne's 5-axis equipment.

• Recommended values are what to design to by default; they keep cost and lead time low.
• Minimum values are achievable but add cost, risk or inspection time; call them out on the drawing.
• Anything outside these limits is not refused outright. Send it for review and Cellborne will confirm feasibility before quoting.
• Dimensions are in inches with metric equivalents. When a drawing and a 3D model disagree, the drawing governs.

Cellborne capabilities

Cellborne machines small precision parts, up to 5 in (127 mm) in the longest dimension, on an automatic 5-axis cell with 100% 5-axis CMM inspection.

The longest dimension of the finished part must fit within 5 in; its thinnest section must meet the material minimum.

• Why plastics need 0.5 in minimum: plastics deflect and move under clamping and cutting heat, so very thin or small plastic parts cannot be held and cut accurately.

Materials

Choose aluminum 6061-T6 unless the application needs something else; it machines fastest and is the lowest-cost option. All materials are sourced traceable from reputable suppliers.

• Specify the exact grade and temper on the drawing (for example "Al 6061-T6"), not just "aluminum".
• Materials not listed can be reviewed on request.

Tolerances & surface finish

Metal parts hold ±0.005 in (±0.13 mm) on size and location and ±0.002 in (±0.05 mm) on hole size; flat metal faces reach 63 µin Ra (1.6 µm). Tighten only the features that need it.

Contoured and side-wall finishes depend on part geometry and tooling; the range shown is typical.

• Untoleranced dimensions are machined to the standard size/location tolerance above. State a title-block default on drawings so there is no ambiguity.
• Tolerance only what matters. Each tight tolerance adds machining passes and inspection time. Mating fits, bearing bores and datum faces deserve them; cosmetic outer faces do not.
• GD&T: define datums on faces that are machined in the same setup as the critical features, and on surfaces large enough for the CMM to probe (≥ 0.125 in / 3 mm wide).
• Plastics expand with temperature and relax after machining; PTFE, UHMW and HDPE may need looser limits than the table shows.
• Finishes: parts ship as machined. Note any cosmetic face on the drawing so tool marks and fixturing are kept off it.

Feature & face accessibility

Every machined feature needs a straight line of sight for a rotating tool from one of the five faces the 5-axis machine can reach in a single setup. The sixth face is held by the fixture.

Faces 1–5 are machined in one setup; the bottom face needs a second. Undercuts are cut with a standard T-slot or dovetail cutter.

• Five faces, one setup. Top and all four sides, plus angled faces and holes, can be machined without re-clamping. This keeps features on those faces accurately located to each other.
• The held face. The bottom of the stock is clamped. Parts that need features on all six faces require a second setup, which adds cost and loosens face-to-face location. Put critical relationships on the five accessible faces.

On the 5-axis machine the part tilts and rotates under a cutting tool that only moves straight down, so five faces are machined in one clamping. The clamped sixth face needs the part flipped into a second setup.

• Tool reach. Keep the line from the spindle to the feature clear of the part itself. Deep features next to tall walls force longer, slower tools.

To cut a boss's round wall, the end mill has to run parallel to the boss. Keep that straight path clear: a shelf, lip or overhang above the boss blocks it, and the boss can't be machined as drawn.

• Undercuts. Avoid them. Where needed, use standard T-slot or dovetail profiles, keep undercut depth ≤ 2× the slot width, and leave open space opposite the undercut of at least 4× its depth so the cutter head can enter.
• Enclosed or internal cavities that no straight tool can reach cannot be machined; split the part into machinable pieces and assemble them, or consider 3D printing.
• Angled features. Holes and faces at compound angles are fine on 5-axis. Give them a flat entry face perpendicular to the hole axis so drills don't walk.
• Workholding stock. Allow material below the part for clamping, which is removed afterward.

Minimum feature sizes

No feature can be smaller than 0.04 in (1.0 mm), Cellborne's minimum feature size; design to the recommended column whenever the part allows.

Deep narrow pockets and tall thin walls force long, slow tools; a generous inside radius lets a larger tool cut the corner.

An end mill is round, so it always leaves a radius in an inside corner. Design that radius in, slightly larger than the tool's, and the corner comes out clean.

A long, thin feature acts like a diving board: the cutter pushes the tip away, it chatters, and it springs back with material left on. Keep pins and bosses within 4× their width, or design support material near the tip.

Holes and threads

Through-holes are cheapest and most accurate; a blind tapped hole needs drilled depth past the last full thread.

• Blind holes have a 118° drill-point cone at the bottom; model them that way, or call out a flat bottom (milled, slower).
• Leave unthreaded depth below a blind tapped hole of at least 0.5× the nominal diameter so the tap does not bottom out.
• Specify threads by callout (for example "1/4-20 UNC-2B × 0.38 deep"), not by modeled helix. Modeled threads are ignored.
• Through-holes are cheaper and more accurate than blind holes; use them where function allows.
• Avoid holes that break out on a curved or angled face; add a spot face or flat.

Edges and corners

• External edges are deburred; call out a chamfer (e.g. 0.010–0.020 in × 45°) rather than an external fillet, which takes a special tool.
• Keep all internal radii in a part the same size where possible so one tool cuts them all.

One chamfer mill cuts any chamfer size by changing its depth. A corner-rounding mill cuts only the radius it was ground to, so each fillet size needs its own tool.

Text, cost drivers & pre-RFQ checklist

Text and markings

• Laser marking is faster and cheaper than engraving; choose it where you can.
• Engrave (recessed) rather than emboss (raised); engraving needs only the text cut, embossing needs everything around it removed.
• Use a bold sans-serif font, stroke width ≥ 0.04 in (1.0 mm), character height ≥ 0.12 in (3 mm), depth 0.010–0.020 in (0.25–0.5 mm).
• Place text on a flat face reachable from one of the five accessible faces.

What drives cost (highest impact first)

1. Number of setups: features on the held sixth face, or that no single orientation can reach.
2. Tall, slender parts: they flex like a diving board under cutting load and may need extra setups or support material.
3. Tight tolerances and tight finishes beyond the standard values.
4. Small tools: tiny corner radii, deep narrow pockets, small threads.
5. Material: stainless, alloy steel and PEEK/ULTEM cost more to buy and to cut than 6061 or acetal.
6. Thin walls and slender features that force light, slow cuts.
7. External fillets: each radius needs its own special tool, so choose chamfers where you can.

Before you submit an RFQ

• Part fits within 5 in (127 mm) longest dimension, and meets the minimum shortest dimension (0.125 in metals / 0.5 in plastics).
• Material grade and temper are specified.
• No feature, wall or hole is smaller than 0.04 in (1.0 mm).
• Internal corner radii are ≥ 1/3 of pocket depth and not smaller than 0.02 in.
• Every feature is reachable in a straight line from the top or one of the four sides.
• Tight tolerances are applied only to functional features; a default tolerance is in the title block.
• Threads are called out on the drawing, not modeled.
• Cosmetic faces are marked.
• 3D model (STEP preferred) is attached; a drawing is included when tolerances, threads or finishes are critical.