Enclosure work comes through this shop every week, and it's the one category where the drawing tells me almost everything I need to know before I look at the material block. A machined aluminum enclosure is a box. It has walls, mounting holes, maybe some tapped threads, a cutout or two for connectors. The parts are simple. The engineering is in the details nobody writes down: how thin the walls actually are, what happens to those walls when you anodize, and whether the flatness callout on the cover is realistic at the size you specified.
This guide is for the engineer who has an enclosure design in SolidWorks and needs to send it to a CNC shop with confidence. It covers the alloy choice that actually matters, wall thickness limits, the tolerances we can hold, what anodizing does to your dimensions, and how quantity changes the price. If you are a CNC machining supplier in China, some of this will look familiar. If you are the buyer, read it before you hit send on the RFQ.
The alloy question: 6061 is the default for a reason
Most enclosure drawings I see specify 6061-T6. That is the right answer most of the time, and it is worth understanding why before you pick something else.
| Alloy | Temper | Strength | Machinability | Anodizing appearance | Typical use |
|---|---|---|---|---|---|
| 6061 | T6 | Good | Excellent | Uniform, bright | Default for enclosures, frames, housings |
| 6063 | T5/T6 | Lower | Good | Excellent, smooth | Extrusions, thin sections, architectural |
| 7075 | T6 | Highest | Good | Darker, uneven | Structural brackets, aerospace, high load |
| 5052 | H32 | Moderate | Fair | Good | Sheet stock, formed parts (not machined) |
| 5083 | H32 | Moderate | Fair | Good | Marine, welded fabrications |
6061 machines cleanly, holds tolerances well, and anodizes to a consistent finish. 6063 is softer and extrudes beautifully, which is why it dominates the enclosure market. Most off-the-shelf enclosure profiles are extruded 6063, then machined. If you are designing a custom enclosure, starting with 6061-T6 bar or plate is the safe call. If you plan to machine from a standard enclosure profile, you are already on 6063 and should design for its lower strength.
7075 is stronger (roughly 30% higher yield than 6061-T6), but it costs more and anodizes darker with more variation. I see 7075 specified for enclosure walls that carry mechanical load. Nine times out of ten, 6061 would do the job and save money. When strength matters, put a finite element analysis on the drawing with the load case; a good shop will discuss it with you before quoting.
Wall thickness: how thin can you actually go
The most common mistake in enclosure design is drawing a wall that looks fine in CAD and machines like a potato chip. Thin walls are not a tolerance problem, they are a rigidity problem. When the cutter pushes on a thin wall, the wall pushes back. The result is a wall that is thicker at the base and thinner at the top, or a wall that vibrates and leaves chatter marks.
Here is what we can do consistently on a production run:
| Wall thickness | Maximum unsupported height | What you get |
|---|---|---|
| 3 mm and above | 150 mm+ | No special handling, standard machining |
| 2 mm | 80 mm | Standard machining, minor deflection control |
| 1.5 mm | 50 mm | Fixturing care, lighter cuts |
| 1 mm | 30 mm | Dedicated fixtures, reduced feed, longer cycle time |
| 0.5 mm | 20 mm | Prototype only, high risk, significant cost |
That "maximum unsupported height" column is the number nobody thinks about. A 1 mm wall that is 10 mm tall is easy. The same 1 mm wall at 60 mm tall is a different animal entirely. The shop cannot fix that in post-processing; it has to be designed around.
If your design has thin walls, three things help, in order of cost:
- Ribs and bosses. A stiffening rib on the inside of a long thin wall costs almost nothing and removes most of the deflection problem.
- Reinforcement in the design. Make the wall thicker at the base where the stress is highest, taper toward the top. Casting-style draft is not needed for machining, but a tapered wall machines cleaner than a straight one at thin section.
- Accept the cost. A 1 mm wall on a 40 mm tall enclosure face is doable; it just adds cycle time and requires a shop that understands fixturing. Budget for it.
Tolerances: what we hold on enclosure features
Enclosures have three tolerance zones, and they are not created equal. Confusing them is where quotes come back high.
| Feature | Tolerance we hold | What it means |
|---|---|---|
| Outside dimensions (length, width, height) | ±0.1 mm | The box size. Easy, standard. |
| Mounting hole positions | ±0.05 mm | Hole-to-hole spacing. Standard for CNC. |
| Tapped threads | Class 2B or better | Thread pitch diameter. Standard. |
| Mating surfaces / cover faces | 0.05 mm flatness | This is where cost starts to climb. |
| Precision bores (bearing fits, alignment) | ±0.01 mm | Only on specific features, not the whole part. |
The flatness callout is the one that surprises people. A cover plate that is 100 mm x 100 mm and 5 mm thick can hold 0.05 mm flatness without much trouble. Make that same cover 300 mm x 200 mm and 3 mm thick, and holding 0.05 mm flatness requires stress relief and careful machining sequence, and it costs more. The tolerance does not scale with size; it scales against it.
My honest advice: put ±0.01 mm only where you actually need it. On an enclosure, that is almost never the entire part. It is one bore, one alignment feature, one mounting interface. Everything else at ±0.1 mm and ±0.05 mm keeps the part manufacturable and the price sane. When I see a print with ±0.01 mm on every dimension, I know I am quoting against an inexperienced drafter, and I will price it accordingly.
What anodizing does to your dimensions
Anodizing is the default finish for aluminum enclosures, and it is where dimensional surprise lives. The oxide layer grows outward from the surface, roughly half of it. A 25μm (0.001 inch) anodize layer adds about half that, 12μm, to each surface. On a 1 mm internal wall, that is the difference between a tight fit and no fit at all.
The full detail is in our aluminum anodizing guide, but the enclosure-specific version is:
- Type II (clear or dyed, 5-25μm): The standard. Fine for cosmetic and light-protection enclosures. Dimensional effect is small but real; a mating cover that slides into a groove needs a few microns of clearance built in.
- Type III (hardcoat, 25-100μm): For enclosures that see wear or outdoor service. The oxide is much thicker, and threaded holes genuinely shrink. A M4 thread with 50μm hardcoat needs the tap size accounted for, or the screw will not go in.
- Masking: Threads and precision bores can be masked before anodizing. That adds a fixture and a process step, so it adds cost. Say on the drawing which features need to stay bare.
For a two-piece enclosure where the cover fits into a recess in the body, the recess needs clearance for the anodize layer on both surfaces. Design the groove 0.05-0.1 mm oversize if you plan to anodize both halves. That single number saves a round of rework more often than anything else in enclosure manufacturing.
Surface finish on machined surfaces
Anodizing does not hide machining marks. If you want a uniform satin look before anodizing, the part needs a surface treatment first. The two options are bead blasting and a finer machining pass.
- Bead blast then anodize: The standard "matte black enclosure" look. Bead blasting with 100-150μm glass bead gives a consistent 0.8-1.6μm Ra surface that anodizes to a uniform satin. Costs a bit more than straight machining, worth it for anything customer-facing.
- Machined finish only: Fine for internal or utility enclosures, but 6061 machining marks are visible and can look uneven after clear anodize.
- Polished then anodize: Rare for enclosures. Polished aluminum shows every fingerprint and scratch. Spec it only if the aesthetic genuinely demands it.
How quantity changes the price
Enclosure pricing is dominated by setup, not by the parts. A typical aluminum enclosure has a program, fixtures, and inspection plan that cost the same whether you machine 5 or 500. The per-part price falls as that setup amortizes.
Here is a rough picture for a medium-complexity enclosure, roughly 150 x 100 x 50 mm, 6061-T6, machined from plate, Type II clear anodize, standard tolerances:
| Quantity | Setup share per part | Relative per-part cost | Notes |
|---|---|---|---|
| 1-5 | High | 5-8x baseline | Prototyping. The program dominates. |
| 10-20 | Medium | 2-3x baseline | Validation runs. Fixture cost spreads thin. |
| 50-100 | Low | 1.2-1.5x baseline | The sweet spot for most enclosure jobs. |
| 200-500 | Low | 1x baseline | Near-optimal. Setup fully amortized. |
| 500+ | Negligible | 0.8-0.9x baseline | May move to casting or extrusion instead. |
The practical insight: an enclosure that is going to 100 units is a machining job. An enclosure going to 5,000 units should at least get a conversation about whether casting the body and machining the faces is cheaper. We machine parts that were cast; we also tell customers when their quantity justifies the casting route. Getting an accurate quote depends on you knowing your real quantity, not the ideal one.
What to send when you request a quote
The difference between a one-day quote and a three-day quote is almost always the drawing. For an enclosure, send:
- The STEP file, not just a PDF. STEP preserves the exact geometry and lets us check wall thickness, draft, and feature sizes in the CAD model.
- A PDF with the tolerance block and finish callouts. STEP does not carry GD&T reliably. The PDF is where we read flatness, position, and surface finish.
- The quantity. Real quantity, even if it is an estimate. A "this might be 20, might be 200" answer produces a quote we both regret.
- The anodizing spec. Type II or III, color, and which features (if any) need masking.
A complete package like that lets us quote accurately the first time. If the drawing is missing tolerances, we will still quote, but we will have to guess, and the price will carry the uncertainty.
Have an aluminum enclosure in development?
Send us your STEP file and drawing. We will review manufacturability, flag the thin walls and tight tolerances before you commit to production, and give you a quote based on the actual machining time. Upload your drawing for a free DFM review and quote. If the design has issues, we will tell you before you spend money on them.
For more context on the aluminum side, see our aluminum CNC machining complete guide and the aluminum part design guide. Both cover the same material with the design engineer in mind. For the cost side, our cost reduction guide covers the levers that actually move enclosure pricing.