The right DMLS machining allowance is 0.5-0.8mm of stock on datums, 0.4-0.6mm radial on bores, and 0.3-0.5mm on sealing faces — added in CAD before the part is ever sliced. Get those numbers right and an as-built print that holds our standard ±0.1mm tolerance can be clamped once, machined once, and shipped inside ±0.05mm without a second setup. Get them wrong and you either machine through the skin into porous sub-surface material, or you leave so much stock the part rocks on its datums and every downstream dimension drifts. At Layer X, having shipped 2,000+ metal parts from our Ahmedabad facility, we plan the allowance at quoting — not after the part comes off the plate — and this is how we decide where the stock goes.
Why as-built DMLS parts need machining allowance at all
Direct Metal Laser Sintering builds Ti-6Al-4V, 316L stainless, Inconel 625, Inconel 718 and AlSi10Mg by fusing 30-60µm powder layers with a laser. The process is remarkably accurate for a near-net technique — Layer X holds ±0.1mm on general geometry — but three physical realities mean critical features can never come straight off the plate to a fit-class tolerance:
- Surface roughness. As-built vertical walls sit around Ra 6-12µm; down-facing surfaces built over support are coarser still. A bearing bore or an O-ring gland needs Ra 0.8-1.6µm, which only machining or grinding delivers.
- Thermal distortion. Every layer shrinks as it cools, so long unsupported spans bow and thin walls pull inward. The part is dimensionally sound but not flat enough to seat on a raw datum.
- Support witness marks. Down-facing features and overhangs below roughly 45° carry support structures. Where those supports break away they leave nibs and a rough scar — never a surface you can seal or reference from.
Machining allowance is simply extra material grown onto these features in CAD so that after heat treatment and support removal there is clean, dense stock for the cutter to remove. ASTM F3301, the standard practice for post-processing metal parts made by powder-bed fusion, treats machining and stress relief as an integral part of the build route rather than an afterthought — and so do we.
The one-setup principle: datums first
The whole discipline of allowance planning exists to serve one goal: finish the part in a single machining setup. Every time a part is unclamped and re-fixtured, you introduce a repositioning error that stacks on top of your machine tolerance. A part that needs three setups to hit ±0.05mm is a part that will argue with its own inspection report.
The way out is to establish a datum reference frame early and never lose it. We nominate a primary datum face (usually the largest flat that other features reference), a secondary edge or bore, and a tertiary stop. Those get the most generous, most reliably dense allowance. Everything measured from them — bores, faces, threaded bosses — is then cut in the same clamping while the datums stay seated on the fixture. As-built, our parts hold ±0.1mm, which is comfortably inside the stock envelope below, so the cutter always finds material where the CAD said it would.
How to orient the part on the plate to protect datums
Build orientation decides how much distortion and support your datums inherit. We orient so that primary datum faces build either vertically or up-facing — never as a down-facing surface hanging over support, where the scar and the extra roughness eat into your allowance. This is the same orientation logic covered in our support structures design guide, applied specifically to the surfaces you intend to reference from.
How much stock to add, feature by feature
These are the starting allowances we quote against for DMLS parts across the metal alloys we run. They assume standard stress relief on the plate before wire-EDM removal, and they are per-surface (a bore machined all round gets the radial figure on every side).
| Feature | Recommended allowance | Why this figure |
|---|---|---|
| Primary datum faces | 0.5-0.8mm | Absorbs distortion plus the coarse skin; gives a clean seat that every other feature references. |
| Bores and bearing bores | 0.4-0.6mm radial (0.8-1.2mm on diameter) | Removes the as-built taper and roughness; leaves dense material for a fit-class finish. |
| Sealing / O-ring faces | 0.3-0.5mm | Flat, up-facing surfaces distort least; enough to reach Ra 0.8µm without over-cutting. |
| Threaded holes (tapped) | Drill/tap solid or leave 0.3mm on a pilot | As-built holes are undersized and rough; cut threads always, never print-to-size. |
| Mating flanges / joint faces | 0.4-0.6mm | Covers edge roll-down and keeps assembly gaps predictable. |
| General non-critical surface | 0mm (leave as-built) | Adding stock you never machine only adds cost, powder and print time. |
Two rules sit behind the table. First, only add stock where a drawing callout demands it — a surface with no tolerance tighter than our as-built ±0.1mm should be left alone. Second, never leave less than the roughness depth plus the local distortion, or the cutter will skim high spots and dig into porous valleys, exposing sub-surface porosity that no amount of polishing hides. For a deeper treatment of what the base process holds before machining, see our tolerances and dimensional accuracy guide.
Support removal comes before machining, not after
Sequence matters as much as stock. A DMLS part that is machined while still supported, or before stress relief, will spring the moment it comes free and throw away every micron you just cut. Our fixed route is:
- Stress relief on the plate. The part is heat-treated while still fused to the build plate, so it relaxes before anything cuts it loose. This is where most of the residual stress leaves the part.
- Cut off the plate (wire-EDM or bandsaw), then remove supports. Manual break-off for accessible supports; wire-EDM for dense support fields under datum faces.
- Solution/age or HIP if specified for the alloy and application — Ti-6Al-4V and Inconel aerospace parts frequently require it.
- Machine the allowance against the now-stable datums, in one setup wherever the geometry allows.
- CMM inspection — supplied with every DMLS order as standard, not as a paid extra.
Getting supports off cleanly without bruising the reference surfaces is its own craft; our clean support-removal guide covers the techniques we use on the shop floor.
Alloy-specific adjustments
The base table is a starting point; the metal changes the details.
- Ti-6Al-4V — low thermal conductivity means more localised distortion, so we lean to the upper end (0.7-0.8mm on datums). Titanium also work-hardens, so generous, consistent stock lets the cutter take one clean pass rather than rubbing.
- Inconel 625 / 718 — tough and abrasive; leave enough stock (0.6mm radial on bores) that finishing passes stay in dense material, and expect slower feeds. HIP is common for these, and HIP shrinks the part slightly, so allowance is planned after the HIP allowance is known.
- 316L stainless — forgiving and stable; the standard figures apply directly.
- AlSi10Mg — machines easily and distorts less, so sealing faces can sit at the 0.3mm floor. Watch smearing on soft aluminium — sharp tooling, not more stock, is the answer.
Designing the allowance into your CAD
The cleanest way to hand us a machinable part is to model the allowance yourself and flag it, so print and machining shops read the same intent:
- Add the stock as an offset on the specific faces, not a blanket scale on the whole body — a scaled part throws off every un-toleranced feature.
- Model bores undersized by the radial allowance (or as solid stock) so we drill and bore to final size.
- Mark datums and machined faces on the drawing with a machining symbol, and state the finished tolerance and Ra so we know what the surface has to reach.
- Keep a consistent wall thickness under sealing faces — a thin, unsupported wall behind an O-ring gland will chatter under the cutter no matter how much stock sits on top.
If you would rather send the finished-geometry model and let us add the allowance, we do that at quoting — but tell us which surfaces are critical and to what tolerance, or we default to leaving the part as-built at ±0.1mm. For parts that combine printed bodies with machined brackets or plates, our CNC sheet-metal service can finish the mating hardware to the same reference frame.
What good allowance planning buys you
Planned properly, machining allowance is the difference between a part that inspects first-time and one that bounces between print and machine shop. Layer X runs a 99.4% first-pass yield across 2,000+ shipped parts precisely because the stock is decided before the file is sliced, not negotiated after the part comes off the plate. Every DMLS order leaves our AS9100 Rev D and ISO 9001:2015 certified facility with a CMM dimensional report, material certificate and certificate of conformance — so the tolerance you asked for is the tolerance on paper, held in one setup.
Ready to get the numbers right the first time? Explore our DMLS metal 3D printing service from ₹5,000/part, or upload your CAD file for a 24-hour quote and we will plan the machining allowance with you before a single layer is fused.