There is no universal minimum wall thickness that makes a CNC-milled part manufacturable. A short 0.8 mm aluminum rib and a 0.8 mm tall plastic wall are not the same machining problem, and neither should be judged only by one dimension in a design-rule table.
Published CNC design guides often use values around 0.8 mm for metals and 1.5 mm for plastics as recommended starting points, with thinner walls possible case by case. Protolabs Network, for example, lists 0.8 mm for metals and 1.5 mm for plastics as recommended values and explains that thinner walls lose stiffness, vibrate more and reduce achievable accuracy. Protolabs Network CNC design guide.
Treat those figures as process guidance, not a standard or a promise from every machine shop.
Why thin walls become difficult to machine
CNC cutting is not a force-free process. The cutter pushes on the workpiece while removing material. A thick section resists that load. A thin wall behaves more like a spring.
As the wall gets thinner, several effects become more important:
- deflection: the wall bends away from the tool, so the cut does not land where the toolpath expected;
- chatter and vibration: low stiffness makes the wall easier to excite;
- heat distortion: plastics and thin metal sections can move as heat and residual stress are released;
- clamping distortion: a part can measure correctly while clamped and move after release;
- finishing difficulty: tight tolerance or surface-finish requirements may require lighter passes and more time.
That is why the meaningful design question is not only “how thin?” but “how thin, how tall, in which material, with which tolerance, and how will it be supported?”
Wall height matters as much as thickness
A 1 mm wall that is 3 mm high is much stiffer than a 1 mm wall that is 40 mm high. Long unsupported walls act like slender beams.
When reviewing a STEP model, record at least:
- wall thickness;
- unsupported wall height and length;
- material;
- nearby pockets or cutouts that reduce support;
- whether the wall can be supported by stock or sacrificial material during machining;
- tolerance and surface finish on that wall.
CADProps can help inspect dimensions in the CAD dimensions tool, but it does not currently claim to automatically find the minimum wall thickness everywhere in a part or certify machinability.
Material changes the practical limit
Metals and plastics behave differently under the same geometry.
A relatively stiff aluminum wall may tolerate a geometry that is troublesome in a softer plastic. Plastics can also soften with heat and warp from residual stress. Stainless steel or titanium may require different cutting conditions and tool engagement than aluminum even when the wall geometry is identical.
The material specification therefore belongs in the RFQ. Do not expect the STEP geometry alone to establish it. If material information is uncertain, read what a STEP file can contain about material.
Why “0.5 mm is feasible” is not a quote
Some published guides list thinner values as technically feasible. That means a capable process may be able to produce them under suitable conditions. It does not mean every 0.5 mm metal wall is economical, stable or acceptable at your tolerance.
A shop may need to change:
- cutter diameter and stick-out;
- roughing sequence;
- finishing allowance;
- number of setups;
- fixturing or soft jaws;
- whether material is left temporarily to support the wall;
- inspection strategy.
Those changes affect price and lead time. A thin wall can be manufacturable and still be an expensive design choice.
A better DFM conversation with a machinist
Instead of asking only “Can you machine a 0.7 mm wall?”, send the released geometry and state the functional requirement.
For example:
This wall is 0.7 mm nominal, 18 mm tall, 6061-T6 aluminum. The inside face controls fit; ±0.05 mm applies to wall thickness after machining. Can you hold it as drawn, or would increasing it to 1.0 mm materially reduce risk or cost?
That gives the supplier enough context to propose a process change rather than guessing why the wall is thin.
Check the rest of the geometry around the wall
Thin walls rarely exist in isolation. Also inspect:
- internal corner radius: a larger cutter is stiffer and usually needs a larger internal radius;
- deep pockets: long tool reach increases deflection;
- holes near the wall: drilling or interpolation can load a fragile edge;
- threads: thread depth and edge distance can weaken thin sections;
- openings and slots: these can turn one stiff wall into several flexible tabs;
- workholding surfaces: the shop still needs somewhere stable to clamp the part.
Protolabs Network's CNC guidance connects thin-wall limits to workpiece stiffness, tool stiffness, tool access and workholding rather than treating wall thickness as an isolated rule. CNC machining engineering guide.
What to inspect in a STEP file before RFQ
- Open the released model in the STEP viewer.
- Confirm units and one known overall dimension.
- Measure the thin wall at several locations if it tapers or curves.
- Note its height, nearby pocket depth and access direction.
- Send the material, tolerance, quantity and finish with the model.
- Ask the supplier whether the wall drives a special setup or machining sequence.
- If the supplier proposes a thicker wall, evaluate the functional impact before revising the CAD.
The STEP for CNC quote guide covers the rest of the handoff.
Use rules of thumb as filters, not approvals
A published minimum is useful for spotting risk early. It is not a substitute for process planning.
For design review, flag walls that approach a supplier's stated guideline and then look at height, material, tolerance and access. For purchasing, let the actual manufacturer confirm what their machine, tooling and fixturing can hold.
That approach avoids two bad extremes: rejecting every thin wall because a table says so, or assuming a thin wall is safe because another website called the number “feasible.”
Original article: CADProps · https://www.cadprops.com/guides/cnc-minimum-wall-thickness/