3D Printing Design Guide for MJF with HP PA12 Nylon

Multi Jet Fusion spreads a thin layer of PA12 powder across the build bed, then an inkjet array prints a fusion agent onto the areas that will become solid and a detailing agent along the edges of those areas. An infrared pass heats the whole layer. Coated powder melts and fuses; uncoated powder stays loose and supports the part. The bed drops, a new layer is spread, and the cycle repeats.

That loose powder is the reason MJF needs almost no support structure. Overhangs sit on powder instead of on printed scaffolding, so the part comes out of the cake surrounded by a soft bed of unfused material. You still need a way to get that powder out of closed volumes. Trapped powder is the most common reason a design comes back with a note attached.

PA12 fuses into a semi-crystalline structure with low porosity. Parts behave like a tough engineering nylon rather than a brittle resin, and thin sections keep a useful amount of flex. Moisture uptake is real: a dry part and a part that has sat in humid air for a week do not measure the same, and they do not feel the same either.

Multi Jet Fusion earns its place on parts with complex internal channels, lattice or honeycomb cores, and brackets that would need five setups on a mill. Batch size matters too. Because the build envelope fills with nested parts, unit cost drops as the cake fills up, so a run of 50 to 500 similar housings is often cheaper in PA12 than in machined plastic.

The process does not hold metal tolerances. A fit that depends on ±0.05 mm should be designed with clearance, or the mating surface should be machined after printing. Load-bearing threads under 3 mm are a poor choice; use a pilot hole and cut the thread later, or switch to a threaded insert.

Surface texture is grainy and slightly matte. That is acceptable on ducting, covers and fixtures. Visible cosmetic panels usually need bead blasting, dyeing or painting to reach a uniform appearance, and even then the surface will not read as injection molded.

Keep walls at 0.8 mm or above. Thinner walls build, but they warp during cooling and the thickness varies across the part. Regions that carry a bolt load, a snap fit or a repeated bending cycle should be 1.5 mm or more. Very thick blocks are the opposite problem: a 20 mm solid section holds heat, cools unevenly and can bow. Use ribs and pockets instead of solid mass.

Small holes come out undersized. Expect roughly 0.1 to 0.2 mm of shrinkage on the diameter, more on deep holes because unfused powder clings to the wall. Model through-holes at nominal size and plan to drill them if the fit is critical. Blind holes deeper than five times the diameter are hard to clean out.

Overhangs are not a problem in this process. Angles from 0° to 90° build without dedicated support, so a design that was cleaned up for FDM can often be simplified. The real risk sits on flat, unsupported faces facing down toward the build plate: they can curl at the edges when the part cools. Add a chamfer or a small boss pattern to stiffen them.

Living hinges, snap fits and press fits all work in PA12 if you size them for the material. A snap hook needs a 0.5 to 1.0 mm undercut and a lead-in chamfer, and it should flex across a thin section rather than through a thick one. Press-fit pins should be modeled oversized and reamed, because the printed bore will not be round to metal standards.

Threaded inserts are the cleaner route for anything that will be taken apart more than twice. Model a boss with a bore sized for a heat-set insert and keep at least 1.5 mm of wall around it. For low-load joints, a self-tapping screw into a pilot hole works, but expect the thread to loosen after a few cycles.

Finishing changes the dimensions. Bead blasting removes a small amount of surface and dulls sharp edges; dyeing adds no thickness but hides color variation between builds; painting adds a coat that can close a 0.5 mm gap. Decide the finish before you set tolerances on a mating feature, and leave a note on the drawing so the shop knows which surfaces matter.

Send a watertight solid, not a surface mesh. STL, STEP and 3MF all work, and STEP is preferred when the model came from a CAD kernel because it keeps true arcs instead of faceting them. Check the mesh for flipped normals and zero-thickness faces, since a slicer will happily build a broken model and you will only find out at inspection.

Add escape holes to every closed hollow volume. Two holes at opposite ends, 3 to 5 mm across, let the loose powder drain and let blasting media reach the inside. Without them the cavity stays full, the part weighs more than the CAD predicts, and trapped powder can later work its way out through a thin wall.

Nest the parts in the build file when you can. Grouping similar parts in one orientation keeps the thermal history consistent across the batch, which narrows the spread in measured dimensions. If a dimension is critical, mark it on the drawing and ask for it to be checked on the first part rather than on the whole run.