Design for CNC: seven changes that cut an EDC quote

Every one of these is something we have suggested on a real EDC drawing and watched take a meaningful percentage off the quote. None of them change the product a customer would notice.

1. Open up internal corner radii

The most expensive single feature in EDC parts. A 1 mm internal radius forces a 2 mm or smaller end mill. Small tools mean shallow depths of cut, many more passes, high spindle speed, frequent tool changes and a real risk of tool breakage mid-part.

Open that to 3 mm and the shop uses a rigid 6 mm tool and clears the pocket in a fraction of the time.

Rule of thumb: internal radius should be at least one third of pocket depth, and as large as the design tolerates. Nobody has ever picked up a knife and noticed a corner radius.

2. Reduce the number of setups

Every time the part is unclamped, flipped and re-referenced you pay for the operation and inherit the tolerance stack between the two sides.

Design so the part can be machined from one side wherever possible. Where a second side is unavoidable, give it a flat datum face and a pair of features that make re-fixturing repeatable. Three setups on a knife scale is a design problem, not a machining one.

3. Standardise hole sizes and thread types

Six different screw sizes on one part means six tool changes and six tools in the carousel. Consolidating to two or three saves cycle time and reduces the chance of the wrong tool in the wrong hole.

Use standard metric threads. A non-standard thread means a special tap, which is a tooling cost and a lead time.

4. Do not floor pockets deeper than they need to be

Depth drives cost disproportionately because tool reach drives rigidity. A pocket at four times tool diameter needs a longer tool, which chatters, which forces lighter passes.

If a weight-reduction pocket can be 3 mm instead of 5 mm, make it 3 mm.

5. Loosen the tolerances that do not control fit

Covered at length in tolerances and fits, but it belongs on this list because it is the biggest single lever. Three or four tight callouts, everything else general.

6. Avoid thin walls next to deep features

A 1 mm wall beside a 6 mm deep pocket will deflect under cutting load, leaving a wall that is thinner at the top than the bottom and possibly chattered. The fix is either a thicker wall, a shallower pocket, or a sacrificial support that gets removed in a second operation — the last being the expensive option.

If the thin wall is structural to the design, say so and expect to pay for it. If it exists because the CAD happened that way, thicken it.

7. Design the finish in, not on

A part that needs bead-blasting, then masking, then anodizing, then laser marking has four handling operations after machining, each with its own queue and its own chance of a handling mark.

Ask whether the design needs all of them. A stonewashed part with a machined-in texture may achieve the same visual result in one step. Each finishing operation removed is typically a week of schedule and a real reduction in the cosmetic reject rate.

When to do this

Before the CAD is finished. Every item on this list is nearly free to change at model stage and expensive to change after you have approved a prototype.

Send the model when it is roughly right rather than when it is perfect. We will mark up what is costing you money while it is still cheap to move. Related: how to write an RFQ a shop can quote.

Two more that come up constantly

8. Do not specify a surface finish the process will erase.

A fine Ra callout on a face that will be bead-blasted or stonewashed is money spent on a surface that ceases to exist. Specify fine finish only under polish or where a seal runs. See tolerances and fits.

9. Use standard stock thicknesses.

A scale finished at 3 mm machined from 4 mm plate needs one face skimmed. The same scale at 3.2 mm from 4 mm plate needs the same operation but leaves more margin for flatness correction. Meanwhile a part designed at 3.5 mm when the shop stocks 3 mm and 4 mm means either buying an unusual thickness at a lead time penalty or removing a lot of material.

Ask what plate thicknesses are commonly stocked, then design to them. It is free and it occasionally removes weeks.

Features that are expensive for non-obvious reasons

Deep small holes. A 2 mm hole 20 mm deep is ten times diameter — peck drilling, chip evacuation problems, drill breakage risk. If it can be 3 mm, make it 3 mm.

Text machined as geometry. Engraved-as-modelled text with sharp serifs requires a tiny tool and a long tool path. Laser marking achieves the same result in seconds. See laser marking vs engraving vs etching.

Undercuts. Any feature that cannot be reached from the tool’s approach direction needs a special tool, a different setup or a lollipop cutter. Sometimes necessary. Frequently the result of a CAD fillet applied without thinking.

Sharp internal corners on a pocket floor. A flat end mill leaves a radius at the floor corner. Specifying a sharp corner there means a second operation or EDM. Design a floor radius in and it is free.

Tangency requirements between surfaces. A contour that must flow perfectly into another surface can require a much finer stepover and a much longer finishing pass. Visually gorgeous, expensive, and worth doing deliberately rather than by accident.

The fillet trap

Most CAD systems apply a default fillet radius. If that default is small — 0.5 mm is a common default — you have just specified a 1 mm end mill across every internal corner of your part without deciding to.

Check every internal radius before releasing a drawing. Set the default in your CAD to something machining-friendly, 3 mm for example, and reduce it only where the design genuinely needs it. This single habit saves more money over a product line than any other item in this article.

Ask for a DFM review, and actually read it

A design for manufacture review is where a programmer tells you what in your model will fight the process. Many shops offer it free with a quote; some do it and nobody reads it.

The useful output is a list like: this radius forces a small tool, this pocket adds a setup, this tolerance triggers CMM inspection, this wall will deflect. Each item usually has a cheap fix at CAD stage.

Ask for the review to include a cost impact per item where possible. “This radius costs roughly 15 percent” is actionable; “this radius is tight” is not.

Prototype before you optimise

One caveat on everything above: do not spend a week optimising a design you have not held yet.

Make one. Carry it. Half the changes you will make after handling a prototype are about feel and proportion rather than cost, and optimising for machining before you have settled the design means doing the work twice.

The efficient sequence is: rough model, DFM review, prototype, design changes, second DFM review, production. Send the rough model — that is the stage where our comments are worth the most.

These changes belong before the RFQ in the route set out in our guide to custom EDC manufacturing.

FAQ

How much can these changes really save? On a typical first-time EDC part, fifteen to thirty percent is normal, occasionally more. The largest single contributors are usually internal radii and unnecessary tolerances.

Will the shop suggest these if I do not ask? A good one will. A busy one may just quote what you sent, because quoting is faster than consulting.

Does design for manufacture make the part worse? Almost never, if you are choosing which changes to accept. Every item in this article is invisible to a customer. Changes that would affect feel or appearance are yours to reject.

What if my design genuinely needs the expensive feature? Then it needs it, and you pay for it. The point is to pay for the features that matter and not for the ones that arrived by accident.

Should I design for a specific machine? Not at this stage. Design for general good practice and let the shop choose the machine. Designing around one shop’s equipment makes it expensive to move suppliers later.

When is 5-axis worth it? When a contoured part would otherwise need three or four setups. At that point the higher hourly rate is offset by fewer operations and better accuracy between features. Ask for it to be quoted both ways if you are unsure.