How to Make a Stencil With a CNC Machine
To make a stencil with CNC machine work, you cut apertures into a flat sheet and control three things: sheet flatness, cutter diameter, and cutting depth. This guide covers sheet choice, CAM settings, clamping, feeds, and the edge checks that decide whether the stencil works on the first run. It is written for engineers and buyers who need repeatable apertures, not a one-off art piece.
Key takeaways
What makes a stencil a machining job
A stencil is a sheet with openings. Paint, solder paste, adhesive, or powder passes through those openings, so the aperture edge is the working surface of the tool. That single fact drives every decision later: the edge must be square, burr-free, and the same size on part one and part five thousand.
Laser cutting burns a taper into the edge and leaves a heat-affected zone. Hand cutting wanders. When you make a stencil with CNC machine cutting, a rotating cutter shears the material and leaves a near-vertical wall, which matters once aperture widths drop below about 1 mm.
The trade-off is speed. A CNC router is slower per aperture than a laser on a 0.2 mm stainless sheet. It wins when the sheet is thicker than 1.5 mm, when the material is aluminium or plastic, when the aperture wall must be square, or when the same sheet carries milled pockets and locating features.
- 1Good fit0.5–6 mm aluminium, brass, steel, PMMA, POM, FR-4, MDF
- 2Poor fit0.1 mm foil, dense 0402 solder-paste arrays, hundreds of sub-0.3 mm holes
Reading the drawing before you cut
Start from the artwork. PCB work usually arrives as Gerber or as a DXF exported from the CAD layer; signage and industrial masks arrive as DXF or STEP. Check the units before anything else. A file drawn in inches and imported as millimetres produces a stencil 25.4 times too large, and that mistake is common enough to be worth a two-minute check.
Then measure the smallest aperture and the narrowest web between two apertures. The smallest aperture sets the maximum cutter diameter. The narrowest web sets how much material you must leave standing, and it is the number that fails first when the design is tight.
Add a tool-entry allowance. Every aperture needs a plunge point, and a helical or ramped entry inside the opening is safer than a straight plunge. If the aperture is too small to ramp inside, lead in from the scrap side or drill the corners first.
Finally confirm the sheet size against the machine travel. Our large-format machines handle 4,000 × 400 × 150 mm, and the medium platform covers 750 × 1,150 × 550 mm. A stencil longer than the table has to be split, and split lines are usually not acceptable.
Sheet selection by application
Stainless 304 at 0.5–1.0 mm is the default for solder paste and for stencils that see solvent cleaning. It holds aperture size after thousands of print cycles. It also work-hardens at the cut edge, so use a fresh carbide cutter and keep the chipload up rather than dwelling.
Aluminium 6061 at 1.0–3.0 mm suits paint, adhesive, and sandblast masks. It cuts fast and stays flat. 5052 is a little tougher and resists bending better if the stencil is handled often. Soft temper sheet gums the cutter, so avoid fully annealed stock.
Brass and copper are chosen for shielding masks and for wear resistance on abrasive media. POM and PMMA cover chemical masking, and clear PMMA lets an operator see the part underneath. PEEK or carbon fibre sheet is used when the stencil sits in a hot press or a curing oven.
Thickness is a process decision, not a preference. Thicker sheet means a longer aperture wall, which reduces paste release. Keep the aperture-width-to-sheet-thickness ratio above roughly 1.5:1, or the paste will not transfer cleanly.
Turning the artwork into a toolpath
Import the DXF or Gerber into CAM, then set the origin so the sheet corner is your zero. Cut the apertures first and the outside profile last. If you cut the outline first, the sheet loses its stiffness and the remaining apertures chatter.
Set depth of cut to sheet thickness plus 0.05–0.10 mm so the cutter fully clears the material and bites into the sacrificial backing. Use a single finishing pass for thin sheet, or two passes when the sheet is over 2 mm. Climb milling gives the cleaner wall on aluminium and plastic.
Pick the cutter by aperture, not by habit. A 1.0 mm two-flute carbide end mill covers most work; drop to 0.5 mm when apertures are under 2 mm. Keep the flute length short. A long, thin cutter deflects and bows the wall, which shows up as a tapered aperture.
Tabs are worth the extra step. Leave 0.3–0.5 mm tabs on the outside profile so small drop-outs stay in place, then cut them by hand and deburr. Without tabs, a loose part can be grabbed by the cutter and damage the sheet.
How to make a stencil with CNC machine: step by step
Follow the order. Skipping the backing plate or the tabs is the most common cause of a ruined sheet.
- 11. Flatten and clean the sheetWipe both faces with IPA and check flatness on a surface plate. Any bow over 0.2 mm across 300 mm will change depth of cut. Do not cut bowed stock.
- 22. Mount on a sacrificial backingFix the sheet to MDF or a plastic board with vacuum, or clamp it around the full perimeter. Small clamps in the middle bend the sheet. Backing also protects the machine table.
- 33. Set the origin and touch offZero X and Y at a known sheet corner. Touch off Z on the sheet surface at the corner, then re-check at the centre. If the two readings differ by more than 0.05 mm, re-clamp.
- 44. Verify the toolpath in airRun the program with Z raised 20–30 mm above the sheet. Watch the rapid moves and confirm no path crosses a finished aperture. Air running catches clamp crashes before they cost a sheet.
- 55. Cut the aperturesSpindle 12,000–18,000 rpm for a 1.0 mm carbide cutter in aluminium; feed 300–600 mm/min; chipload 0.01–0.02 mm per tooth. Drop feed on the first aperture if the sound changes.
- 66. Cut the outline last with tabsLeave 0.3–0.5 mm tabs every 50–80 mm around the profile. Cut them with a deburring tool afterwards. Never let a loose part free itself inside the machine.
- 77. Deburr and inspectBreak both edges with a fine stone or a 400-grit lap. Inspect aperture size on a vision system or an optical comparator, then check flatness again after deburring.
Which cutting route fits the stencil
Aperture width is measured at the narrowest point. Sheet thickness is the finished thickness.
| Stencil condition | CNC mill or router | Laser cutting | Notes |
|---|---|---|---|
| Sheet over 1.5 mm thick | First choice | Slow, heavy dross | CNC holds a square wall |
| Aluminium, brass, POM | First choice | Reflective or gassy | Better chip control on CNC |
| Apertures under 0.3 mm | Not practical | First choice | Cutter diameter is the limit |
| Square aperture wall needed | First choice | Tapered edge | Matters for paste release |
| Sheet under 0.5 mm steel | Possible with care | First choice | Clamping is the risk |
| Mixed pockets and holes | First choice | Not possible | One setup, one sheet |
Symptom, cause, and fix
| Symptom | Likely cause | Fix |
|---|---|---|
| Aperture oversize by 0.05 mm | Cutter runout or deflection | Re-chuck, shorten flute length |
| Tapered aperture wall | Long thin cutter bowing | Reduce flute length, lighten feed |
| Burr on one side only | Climb vs conventional mismatch | Cut all apertures one direction |
| Sheet vibrates and chatters | Gaps under the sheet | Add backing, re-clamp edges |
| Part lifted during cut | No tabs on the profile | Add 0.3–0.5 mm tabs |
| Apertures shifted on the sheet | Origin set from a bowed corner | Re-zero after re-clamping |
When to cut, when to etch
If the sheet is 1 mm or thicker and the wall must be square, make a stencil with CNC machine cutting. If apertures are under 0.3 mm in thin foil, etching or laser is the honest answer, and we will say so before you order.
Questions engineers ask
Can I make a stencil with CNC machine on a 0.2 mm stainless sheet?
It is possible but unforgiving. The sheet flexes under cutting force, so you need full vacuum support, a sharp 0.5 mm cutter, and light passes. Below 0.2 mm most shops move to chemical etching or laser cutting instead.
What tolerance can I expect on aperture size?
With a rigid setup and a fresh carbide cutter, ±0.02 mm on aperture size is realistic on aluminium and brass. On 0.5 mm stainless the practical window is wider because the sheet moves more. Our general machining tolerance is ±0.005 mm where the geometry allows.
How many passes for a 3 mm aluminium stencil?
Two or three. Take the bulk in the first pass at 60–70% of cutter diameter, then finish with a light pass. Single-pass cutting at that thickness loads the cutter and pushes burrs onto the exit edge.
Should I mirror the artwork?
Only if the stencil is used from the opposite face. Most stencils are cut as drawn and used face-up. State which face is the working face on the drawing, and mark it, so the shop does not guess.
What finish should the stencil have?
Usually none. A deburred edge is enough for paint and paste. If the stencil sees abrasive media or frequent cleaning, anodizing on aluminium or a light bead blast helps. Laser marking can add part numbers at a minimum character height of 1.5 mm.
Can you cut the stencil and the fixture in one setup?
Yes, and it is often the better route. Cutting the stencil and its locating plate from the same program keeps the apertures aligned to the fixture features. Send both sets of geometry in one file with a shared origin.
Send the artwork, get a DFM check in 12 hours
Upload the DXF, Gerber, or STEP file and we return a quotation plus a free DFM analysis within 12 hours. Uploads stay confidential and an NDA is available on request.
12-hour quote100% inspectionNo minimum order quantity
More from the shop floor
We publish setup notes, tooling trials and inspection data from the factory floor.
