Key decisions
- Review tool and holder access together, including the surfaces used for clamping.
- A corner-radius change can help more than a blanket tolerance relaxation.
- Approve each geometry change against the mating component and drawing revision.
Review the part as a sequence of reachable surfaces
Design for manufacturability in CNC machining starts with access. A feature that looks straightforward in a transparent CAD view may sit behind a wall, beneath an overhang or beyond the reach of a sufficiently rigid tool. The cutter needs to reach the material, the holder needs clearance, and the part still needs a secure place to be held.
Rotate the model through candidate setup directions and identify what becomes inaccessible in each position. Include drill entry and exit, thread-tool clearance and the space required to remove burrs. A design review that stops at the main milling operation can miss the manual or secondary work needed to deliver an acceptable component.
DFM is also an approval process. A supplier may suggest a larger corner radius, a through hole or a different stock form, but the responsible designer decides whether the change preserves fit, strength, appearance and serviceability. Record proposals separately from the released drawing so an apparently helpful change cannot become an undocumented requirement.
Treat pocket depth and corner radius as one problem
A small internal corner can force a smaller finishing tool. When that corner lies deep inside a pocket, tool reach becomes equally important. Sandvik identifies tool overhang and system rigidity as contributors to vibration; its corner-milling guidance also explains why increased engagement through a corner requires attention. The design implication is to review radius, depth and access together.
A larger radius is useful only if the assembly permits it. A square mating block may require corner relief instead, or the pocket may need a different manufacturing approach. Do not enlarge the radius merely to match a convenient cutter without checking the mating part. Likewise, a cutter whose radius exactly equals the internal radius may have a more difficult path than a smaller cutter with room to interpolate.
| Design condition | Possible approved revision | Verification before adoption |
|---|---|---|
| Deep pocket with very small internal corners | Increase corner radius or add local corner relief | Check the mating shape, fastener access and remaining wall section |
| Tall unsupported wall | Add a rib, shorten the free span or retain machining support | Check assembly clearance, mass and the final free-state shape |
| Blind feature below an overhang | Change entry direction or split the component | Assess added joints, sealing interfaces and assembly work |
| Several unrelated pocket depths | Standardize depths where function allows | Confirm remaining material and local clearances |
| No suitable gripping surface | Allow a temporary holding feature or revised blank | Define its removal and the final inspection state |
Worked example: a deep pocket with tight corners
Consider an illustrative 40 × 30 mm pocket, 20 mm deep, initially drawn with 1 mm internal corner radii. These dimensions support a design exercise for comparing tool access, not a universal machining limit.
An approved larger corner can change the finishing strategy without changing the pocket floor or mounting-hole positions. By contrast, relaxing an unrelated outside dimension would leave the difficult feature untouched. Good DFM therefore links each change to the operation it simplifies instead of treating every drawing tolerance as a cost problem.
Identify what the radius change actually buys
Reaching an R1 corner requires a tool radius no larger than 1 mm for conventional end milling. A nominal 2 mm cutter therefore faces a depth-to-diameter ratio of 10 before allowance for holder clearance. If the mating component permits R4.5 corners, an 8 mm cutter becomes a candidate, with a pocket-depth-to-diameter ratio of 2.5 and room for a curved toolpath. This does not prove that one tool can perform every pass, or that the smaller cutter is impossible. It identifies why the revised geometry deserves a process comparison. The supplier must still assess cutting length, neck geometry, holder collision and chip removal.
Check the shape after the fixture releases it
A thin wall can deflect during cutting or clamping and return toward a different shape when the load is removed. The risk depends on unsupported height, material, geometry, cutting direction and holding method. A single published minimum-wall number cannot describe every combination. Ask how the finished requirement will be assessed in the relevant free or restrained condition.
Removing a large volume from one side of a blank may also make dimensional stability a route-planning concern. Material condition, stock preparation and roughing sequence belong in that discussion. Extra material or an intermediate operation may be justified, but should not be added to every design by default.
Inspection access deserves the same review as cutting access. A narrow internal ledge may be reachable by a tool yet difficult to probe with the intended measurement system. If the feature is functionally important, define an accessible inspection method or reconsider the geometry before release.
Make the DFM review actionable for purchasing
Send both the model and the controlled drawing to Beigain, then distinguish mandatory interfaces from negotiable geometry. A clear response can identify the original feature, the proposed change, its manufacturing reason and the functional approval needed. This is more useful than a generic statement that the part is complex.
Request a revised quote only after the design change is defined. A lower price based on an unspecified radius, alternate material or deleted inspection requirement is not a like-for-like saving. Retain the accepted DFM record with the purchase order so repeat batches do not reopen decisions that have already been resolved.
- Check every deep feature for cutter, neck and holder clearance.
- Review internal radii against the mating component rather than the CAD appearance.
- Identify thin walls and specify the relevant inspection restraint condition.
- Confirm thread exits, cross-hole burr removal and edge treatment.
- Show which surfaces may be used for holding and which must remain cosmetic.
- Separate optional revisions from mandatory dimensions and document approvals.
- Update the model, drawing and quotation to one released revision.
Questions about this topic
Is there a universal maximum pocket depth for CNC milling?
No. Depth interacts with cutter diameter, reach, material, holder clearance and surface requirements. A supplier should evaluate the actual feature rather than apply a single depth limit to every design.
Should all internal corners use the same radius?
Standardizing radii can simplify planning where function allows it. Different radii may still be necessary for mating geometry, stress distribution or local access. Approval should follow the design requirement.
Can a sharp internal corner be machined with a rotating end mill?
A rotating end mill leaves a radius in an internal planar corner. If a truly sharp corner is essential, discuss relief geometry or a suitable additional process instead of assuming conventional milling can create it.
Does a DFM suggestion authorize a supplier to change the part?
No. Treat it as a proposal until the drawing authority approves the revision. The accepted change should be reflected in the manufacturing documents and purchase order.
Technical references
- Sandvik Coromant: Milling inside corners — Primary guidance on cutter engagement and corner toolpaths; design changes in this article require purchaser approval.
- Sandvik Coromant: How to reduce vibration in milling — Primary guidance on overhang, rigidity, workholding and vibration. The pocket dimensions are an original illustrative example.
Continue reading
- CNC Milling Services
- Aluminum Machined Parts
- Preparing a CNC RFQ that suppliers can quote accurately
- Request a Manufacturing Quote
READY TO SOURCE YOUR PART?
Get a machining quote for your drawing.
Send your drawing, material and quantity. Beigain reviews the machining features, finish and inspection requirements with your quotation.
Upload drawing for a quoteDownload the RFQ checklist (PDF)
