CNC Machined Aluminium Profile 40 x 40 mm Drilled and Tapped Cut List

01What can a machined aluminium profile actually hold?

Three different tolerances live on a machined 40 x 40 mm aluminium profile, and they come from three different operations. Confusing them is the root of most arguments about a batch that “does not fit”. The cut length comes from a saw, the hole pattern comes from a jig or a machining centre, and the section itself comes from the extrusion die — and the extrusion die is the loose one.

Read that table the other way round and it becomes a design rule: anything tighter than the section tolerance cannot be referenced to the section. If a hole has to sit within 0.1 mm of a face, that face has to be machined first, and the hole is then located from the machined face. Without that sequence the tolerance is aspirational.

02Where does the datum come from?

Not from the extruded surface. An extruded face carries twist and bow that are entirely legal under the extrusion standard but far outside any machining tolerance, and a part located from that face inherits all of it. This is the single most common reason a first batch is rejected: the drawing dimensioned everything from a face that was never flat.

• Machine one or two adjacent faces and call them out as datum A and B. Two adjacent faces remove five of the six degrees of freedom and give a stable setup.
• Keep the machined face away from the slot mouth. Machining across the mouth leaves a burr inside the slot that a T-nut will find on the first assembly.
• Do not use the slot itself as a datum unless the drawing says which face of the groove, because the groove has two and they are not the same.
• For repeated parts, add a jig bore. One 6 mm hole machined in the same setup as the pattern becomes the reference for every subsequent operation, and it makes re-work possible instead of scrapping the part.

03How deep can you tap, and where?

This is where profile machining differs from machining a solid block. A 40 x 40 mm four slot section weighs between 1.30 and 2.35 kg/m depending on wall, which puts the standard wall at roughly 2 mm and the heavy wall at roughly 3.5 mm. Those are estimates from the mass, not drawing dimensions — check the actual section drawing before committing a thread.

The honest summary: a thread in a 2 mm wall is a location, not a fastening. It will hold a cover in place and it will strip the first time somebody over-tightens a bracket. Every load-bearing connection on this section should go through the slot with a T-nut, through the centre bore, or right through the section with a nut on the far side.

04What does batch consistency actually mean?

It means the 500th part is the same as the first, and it is a process question rather than a tolerance question. Four things drift across a batch, and each has a different control.

The control that actually works is boring: a first article inspection on every re-setup, with a signed dimensional report, and a sample check at the end of the run. It costs a few parts and it converts a whole class of complaints into a conversation about a report instead of a photograph.

05How should the drawing be prepared?

A cut list in a spreadsheet is enough for cutting only. The moment there are holes, the drawing has to carry them, and the format matters less than the content.

• Send DWG, DXF, STEP, IGES or PDF. We work in all five. A STEP model plus a PDF with the tolerances is the combination that produces the fewest questions.
• Give one drawing per part number, not one drawing with a table of variants. Variants in a table are where the wrong hole pattern gets drilled.
• State the datum faces explicitly with a datum symbol, and say whether they are as-extruded or machined.
• Dimension hole positions from the datum end, not from both ends. Two reference ends means two tolerances stacking.
• Say what the part does. “Bracket fixing” and “guard panel fixing” produce different decisions about thread depth and edge distance, and a shop that knows the function will flag a bad callout instead of building it.
• Mark the visible faces. It decides which face gets the machining marks and which face may be used for clamping.

06How is deburring done, and what does it cost?

Every cut and every drilled hole leaves a burr, and on an anodised part a burr is worse than a cosmetic problem — it holds moisture and it cuts the operator. There are four routes and they are not interchangeable.

For a 40 x 40 frame kit the practical answer is brush deburr on the cut ends plus a quick hand pass on drilled holes. That is what most kits ship with. If the parts go for anodising, the deburr has to happen first, because anodising does not hide a burr — it makes it permanent.

07What should not be sent to a profile shop?

There is a category of work where an extrusion-based supplier is the wrong choice, and saying so early saves a rejected batch.

• Tight true-position patterns in thin walls. A bolt circle held to 0.05 mm in a 2 mm wall will move when the part is clamped for machining and move again when it is released. Use a machined plate.
• Deep bores. A bore more than a few diameters deep in an aluminium profile is a specialist operation with a boring bar, not a drilling operation.
• Flatness on a large as-extruded face. If the requirement is a flat plate, start from plate.
• Threads below M5 in a 2 mm wall. There is not enough material for the thread to survive a torque wrench.
• Welded assemblies that must then be anodised. The weld pool is a different alloy from the extrusion, and it anodises to a different colour every time. Bolt it instead.
• Anything needing a material certificate for a specific heat number unless that is raised at enquiry — traceability to heat number is available but it changes the purchasing route.

08Questions from design and purchasing

Related sections and categories

Browse CNC Machining, 40 Series Aluminium Profiles, the 40 x 40 mm four slot section for the base section data, or the framing kit with a cut list if the whole frame is being bought as one package.