Who this guide is for
This guide is for engineers and product designers who are drawing a machined aluminum housing: an enclosure for electronics, a sensor body, a gearbox cover or a manifold block. These parts tend to have pockets on more than one face, angled ports, threaded holes for lids and connectors, and at least one sealing surface. They are also the parts where small drawing decisions have a large effect on how long the part takes to machine and how reliably it meets the print.
The tips below are written around five-axis machining, because that is the most common way to make housings with features on several faces. Most of the advice applies just as well to three-axis work; it simply becomes more important when the part has to be re-clamped several times.
Tip 1: Decide early which faces carry the datums
Before modelling details, decide which surfaces locate the housing in the assembly. Usually that is a mounting face plus two holes or two edges. Put those datums on the drawing and reference every critical feature back to them.
On a five-axis machine the shop can often cut the datum face, the bores that align with it and the sealing face in a single clamping. When the drawing is built around the same datums, the inspection report will measure what the machine actually controlled, and you avoid tolerance chains that look tight on paper but are not functionally needed.
- Choose one primary datum face that is large, flat and machined in the first operation
- Use two holes or two machined edges as secondary and tertiary datums
- Reference port positions and lid holes to these datums rather than to each other
Tip 2: Size internal corners for the tool, not for the CAD default
A milling cutter is round, so every internal vertical corner in a pocket has a radius. If the model shows a sharp corner, the shop has to choose a radius for you, and it may not match the mating part.
Pick a corner radius slightly larger than the cutter you expect to be used. When the radius equals the tool radius exactly, the cutter wraps around the corner and engagement spikes, which can leave chatter marks. A radius a little larger lets the tool arc through the corner smoothly. Keeping the same radius on similar pockets also lets one tool finish all of them.
Typical starting point
For pockets around 10–25 mm deep, corner radii of roughly 3–6 mm are common. Deeper pockets need larger radii because they need longer, stiffer tools.
When a square corner is required
If a square component must sit in the pocket, add relief cuts (often called dog-bone or T-bone corners) instead of asking for a sharp internal corner.
Floor radius
The corner between a pocket wall and its floor follows the tool tip. Square end mills leave a sharp floor edge; bull-nose tools leave a small radius. State which one you need only if it affects fit.
Tip 3: Keep depth and wall thickness in proportion
Deep, narrow pockets need long tools, and long tools deflect and vibrate. As a rule of thumb, depths up to about three to four times the tool diameter machine comfortably. Beyond that, machining slows down and finish quality drops.
Thin walls behave in a similar way. Aluminum housings commonly use walls of about 1.5 mm and thicker for general features. Thinner walls are possible, but they can vibrate during cutting and can move slightly after machining as internal stresses in the stock relax. If a thin wall is needed for weight or space, consider a rib or a thicker lip at the top edge to stiffen it.
| Feature | Comfortable starting point | Notes |
|---|---|---|
| Pocket depth | Up to ~3–4 × tool diameter | Deeper is possible but slower |
| General wall thickness | ~1.5 mm and up | Thinner walls may chatter or move |
| Internal corner radius | Slightly larger than tool radius | Keep consistent across pockets |
| Tapped hole depth | ~1.5–2 × thread diameter of full thread | Deeper threads add little holding strength |
| Hole depth for drilling | Up to ~6–10 × diameter | Deeper holes need special drills |
Tip 4: Use five axes for angled features, not for everything
Five-axis machines can tilt the part or the spindle so that angled ports, chamfers and features on side faces are cut without special fixtures. That is where the process pays off.
Features that are parallel or perpendicular to one face can usually be cut with the part held square, even on a five-axis machine. Positioning the part once and cutting several faces from that position, sometimes called 3+2 machining, is often faster and more rigid than continuous five-axis motion. Reserve continuous five-axis motion for genuinely sculpted surfaces.
Tip 5: Plan threads, inserts and fasteners together
Housings usually have many tapped holes: lid screws, PCB standoffs, connector flanges and mounting points. A few habits keep these reliable:
- Standardise on a small number of thread sizes so fewer tools are needed
- Call out thread depth as usable full-thread depth, not total hole depth
- Leave material below blind threads so the tap does not break through into a pocket
- Consider helical or key-locking inserts where threads will be assembled many times
- Keep holes away from thin walls so tapping does not bulge the wall
Tip 6: Tolerance only what is functional
A general tolerance block such as ISO 2768-m covers most dimensions on a typical aluminum housing. Add tighter tolerances only where the function demands it: bearing bores, dowel holes, gasket grooves, connector cut-outs and mating faces.
Each tight tolerance adds inspection time and can force a slower finishing pass. A drawing where everything is tight tells the machinist nothing about which features truly matter.
If you are unsure what tolerance a feature needs, describe its function on the drawing (for example "seal face for O-ring" or "slip fit for 608 bearing"). That lets the reviewing engineer suggest a sensible value.
Tip 7: Design sealing faces and grooves deliberately
For a housing that must keep out dust or water, the sealing surface deserves its own callouts: flatness on the face, surface finish where the seal touches, and groove dimensions that follow the seal maker's recommendations. Keep fasteners evenly spaced around the seal so clamping load is uniform.
Avoid placing a seal groove right next to a deep pocket or thin wall. Clamping forces during machining and assembly can distort thin sections enough to open a leak path.
Tip 8: Choose the alloy and finish together
For most housings, 6061-T6 is a sensible default: it machines well, anodizes evenly and is widely available as plate and bar. 7075-T6 offers higher strength for thin, loaded parts, but it costs more and its anodized color can be less uniform.
Finishing affects dimensions. Type II anodizing builds a thin layer on every exposed surface, roughly half of it growing outward. For most features that is negligible, but for tight bores and threads it matters. Either mask those features or state whether dimensions apply before or after finishing. Bead blasting before anodizing gives a uniform matte look and hides fine tool marks.
Cosmetic faces
Mark which faces are cosmetic. The shop can then plan clamping and tool paths so that witness marks and step lines fall on hidden faces.
Marking
Part numbers and logos can be laser marked after anodizing, which avoids engraving tools and keeps the mark crisp.
A short pre-release checklist
- Datums defined and critical features referenced to them
- Internal corner radii set slightly larger than the expected tool radius
- Pocket depths and wall thicknesses within comfortable proportions
- Thread sizes standardised and depths stated as full-thread depth
- Tight tolerances limited to functional features, with function described
- Sealing faces called out with flatness and finish
- Material, finish and masking stated, with cosmetic faces marked
Next steps
When the model and drawing are ready, upload the STEP file and PDF drawing through the quote form. An engineer reviews setups, tolerances and finishing before pricing, and will flag features that could be simplified without affecting function.