Practical tips that make your parts easier and cheaper to machine
Small design decisions have a big impact on machining cost and lead time. A part that's designed with manufacturing in mind can be half the price of one that isn't — with no change in function. These guidelines come from decades of quoting and cutting real parts. Apply them early in your design process and you'll get better parts, faster, for less.
The single biggest DFM issue we see on drawings
End mills are round — they physically can't cut a sharp 90° internal corner. Every internal pocket corner will have a radius equal to the tool radius. Designing with appropriate radii lets us use larger, more rigid tools that cut faster and last longer.
Thin walls deflect under cutting forces, causing chatter, poor surface finish, and out-of-tolerance dimensions. The thinner the wall relative to its height, the more problematic it becomes.
A CNC tool can only cut what it can physically reach. Internal undercuts, cavities with small openings, and features hidden behind other geometry add significant complexity.
Every time we flip or re-fixture a part, it adds time and introduces alignment error. Parts that can be completed in fewer setups cost less and hold tighter tolerances between features.
Every surface has a finish — the question is whether you need to control it. Specifying a tight finish on a non-critical surface adds unnecessary time and cost.
The material you choose directly impacts machining time, tool wear, and achievable tolerances. A material swap can sometimes cut your part cost in half with no change in function.
See our full Materials Guide for properties and recommendations →
Issues that come up frequently on customer drawings
Putting ±0.001" on every dimension when only 3 features actually need it. This doubles machining time and inspection cost for no functional benefit.
Designing square internal pockets expecting sharp 90° corners. End mills are round — there's always a radius. Design your mating part to accommodate it.
A 0.060" wide slot that's 1.5" deep requires a long, thin end mill that deflects and breaks. Widen the slot or reduce depth if function allows.
Tolerancing features without specifying which surfaces are datums. We need to know what to set up from — otherwise we're guessing at your intent.
Calling out 16 Ra finish on a hidden surface that bolts to another part. Save the fine finish call for surfaces that seal, slide, or show.
Designing a 2.030" wide part that forces us to buy 2.5" or 3" stock. A 1.990" width machines from 2" flat bar — saving material cost and one facing operation.
Sending a 3D model with no drawing, or a drawing missing critical dimensions. We need explicit tolerances on features that matter — a model alone doesn't tell us what's critical.
A 2" deep pocket with a 0.030" floor deflects and can punch through. If you need a thin floor, reduce pocket depth or add ribs for support.
A clear drawing gets you a faster, more accurate quote
Don't make us guess. Every feature should be dimensioned. Missing dimensions delay quoting while we ask for clarification.
Not just "aluminum" — which alloy and temper? "6061-T6" vs "7075-T6" makes a big difference in price and capability.
If specific surfaces need a particular Ra value, call it out. If anodizing, plating, or coating is needed, note that too.
Per-part price varies significantly with quantity. Give us the quantity (or range) so we can quote the most efficient process.
Part number, revision, material, finish, and general tolerances in the title block keep everything organized and prevent miscommunication.
A STEP file paired with a PDF drawing is the gold standard. The 3D model speeds up programming; the drawing defines tolerances and inspection criteria.
| Feature | Guideline | Why It Matters |
|---|---|---|
| Internal corner radius | ≥ 1/3 pocket depth | Allows larger, faster tools |
| Wall thickness (aluminum) | ≥ 0.040", prefer 0.060"+ | Prevents deflection and chatter |
| Wall thickness (steel) | ≥ 0.060", prefer 0.080"+ | Steel walls resist deflection better |
| Hole depth | ≤ 4x diameter (standard) | Beyond 4x requires peck drilling |
| Thread engagement | 1.5-2x bolt diameter | Full strength without wasted depth |
| Height-to-thickness ratio | ≤ 4:1 (easy), 4-8:1 (careful) | Tall thin walls vibrate and deflect |
| Standard tolerance | ±0.005" | Tighter only where function requires |
| Text/engraving depth | 0.010" - 0.020" | Legible without excessive tool wear |