Ordering from a Fabrication Service
Choosing a service, the options on the form, files, the engineering check and what to inspect on arrival.
Choosing a service
A fabrication service makes boards from your files in a factory and ships them. Services, prices and rules change, so the names here are examples only: check the current ones before you design.
| Type | Examples | Typical strengths | Watch for |
|---|---|---|---|
| Low-cost prototype houses | JLCPCB, PCBWay, ALLPCB, Seeed Fusion | Very low prices for small boards; online quote and preview; assembly and stencils offered | Shipping time and cost; customs; minimum quantity of 5 or 10 |
| Community and hobby services | OSH Park, Aisler, Eurocircuits (Europe) | Good quality, clear rules; shipping within a region; priced by area | Higher price per cm² than the largest houses |
| Domestic quick-turn services | Advanced Circuits, Sierra Circuits, Bay Area Circuits, Würth | Fast delivery and engineering help; tight specifications | Price; minimum order value |
| Full-service manufacturers | Contract manufacturers | Production runs; controlled impedance, rigid-flex; high-reliability classes | Set-up costs; longer lead times |
| Local shops and makerspaces | University or hackerspace | No shipping; hands-on help | Capability varies |
- Match the service to your design rules (trace and space, hole size, layer count): download their rules file and load it into your design-rule check.
- Compare the total with shipping and duty, not the price shown first.
- Read recent reviews for quality and support, and keep the first order small.
- Stay with one service for a project: their rules and stack-ups become familiar.
The options on the form
| Choice | Options | Advice |
|---|---|---|
| Layers | 1, 2, 4, 6 and more | Two for simple boards; four for microcontrollers with USB and for noise (see Layer Stack-up and Impedance) |
| Dimensions | Your outline in mm | Under 100 × 100 mm is the cheapest class |
| Quantity | 5, 10, 20, 30 and more | The first 5 or 10 are nearly the price of the set-up |
| Thickness | 0.6 to 2.0 mm; 1.6 mm standard | 1.6 mm unless a connector or enclosure needs another |
| Copper weight | 1 oz (35 µm), 2 oz | 1 oz for signals; 2 oz for heavy currents |
| Surface finish | HASL (lead-free or leaded), ENIG, OSP | HASL for cheap and coarse parts; ENIG for fine pitch and BGAs (see Manufacturing Rules, Files and Design Review) |
| Solder mask color | Green, black, white, blue, red | Green is the fastest and cheapest |
| Silkscreen | White (usual), black | Check the line width |
| Panelization | Single boards or panel (V-score, tabs) | Ask for a panel if you will assemble by machine |
| Via treatment | Tented, plugged, open | Tented is the usual default |
| Impedance control | None, or specified | Only if the design needs it; they adjust the widths |
| Electrical test | Flying probe or fixture | Include it: it finds open and short circuits |
| Assembly, stencil | Optional | See Assembly: Stencils, Reflow and Assembly Services |
Files and checks before you upload
The service needs Gerber files for each layer and a drill file (see Manufacturing Rules, Files and Design Review for the list). A typical set is 11 files in a zip of about 90 kB for a four-layer board.
| Check | What to look for | If wrong |
|---|---|---|
| Outline | One closed outline on its own layer; correct size; mounting holes and cut-outs present | No or double outline: the service cuts the board wrongly or asks you |
| Drill file | Holes where they should be, right units, plated and unplated separated | Shifted or wrong sizes, from a wrong origin or units |
| Layer count and order | Each copper layer in its own file with a clear name | A swapped layer gives a short or open board |
| Mask and paste openings | Pads open; the mask dam present where it should be | Pads covered, so nothing to solder to |
| Silkscreen | Not over pads; legible | The service clips it or the text is unreadable |
| Mirrored or rotated layers | Bottom layers viewed as from the top | The board is a mirror image |
| Minimum rules | Clean DRC with the service’s rules | The service will adjust, reject or charge more |
| Board size | Compare with the design: Gerber viewers measure | Wrong units (inch for mm) give a tiny or huge board |
- View the files in an independent Gerber viewer (the service’s own preview, or a free one such as gerbv or KiCad’s viewer) and compare each layer with the design.
- Zip the files with a clear name and revision (for example sensor-v2-gerbers.zip).
- Write notes for the service: layer count, finish, thickness, any impedance or special requirement.
Ordering step by step
- 1. Finish the design and run the design-rule check with the service’s rules.
- 2. Export the files (Gerber, drill; BOM and placement if you want assembly) and zip them.
- 3. View the files in an independent viewer.
- 4. Upload to the service and compare its preview of each layer with your own; check the board size shown.
- 5. Choose the options: layers, thickness, copper, finish, mask color, quantity, test, stencil.
- 6. Choose speed and shipping. Express shipping for a deadline; slow shipping for a hobby board.
- 7. Read the final price with shipping and tax or duty, then pay.
- 8. Answer the engineering query quickly: the clock stops until you do.
- 9. Inspect on arrival (below).
Reading a quote
Worked example: pricing ten sensor boards
A 45 × 30 mm two-layer board (13.5 cm²), 10 boards. Using the illustrative model ($5 set-up + $0.012 per cm² for each board; real prices differ):
- Base: 5.00 + 0.012 × 13.5 × 10 = $6.62 for the boards.
- Shipping $14.00 brings the subtotal to $20.62. With 10 % tax or duty (varies by country) the total is $22.68, i.e. $2.27 per board.
- Adding ENIG and black mask: $32.58 in all; as a four-layer ENIG version: $38.02.
- Shipping and tax were 71 % of the basic order: for small orders they dominate, so order enough and do it once.
| Option | Extra cost (model) |
|---|---|
| Two layers, 1.6 mm, HASL lead-free, green | included in the base |
| ENIG finish | +$6.00 |
| Black solder mask | +$3.00 |
| Four layers (instead of two) | +$7.94 |
| Express production, 24 h | +$9.93 |
| Stencil, 0.12 mm, framed | +$8.00 |
| Controlled-impedance report | +$4.00 |
Lead time
Worked example: days to the first board
- Prepare and check files 1 d, Engineering review by the service 1 d, Fabrication (standard) 4 d, Shipping (express) 5 d, Customs and delivery 1 d: a total of 12 days with express shipping.
- With ordinary post (14 days instead of 5) it is about 21 days. Always allow a week more than the quote for problems.
- Assembly adds parts sourcing and a week or more (see Assembly: Stencils, Reflow and Assembly Services and Cost, Quantity and Lead Time).
Inspecting boards on arrival
Worked example: what to check and the allowed tolerances
- Outline: measure with calipers: 45 × 30 mm ± 0.2 mm.
- Thickness: 1.6 mm ±10 % = 1.44 to 1.76 mm.
- Holes: finished 0.8 mm ± 0.1 mm: the lead of the part must fit, so check the smallest part that goes in a hole.
- Bow and twist: for surface-mount boards IPC allows 0.75 % of the diagonal or length (0.34 mm over the 45 mm edge); 1.0 % for through-hole boards (0.45 mm). Lay the board on a flat surface and check with feeler gauges.
- Electrical: a flying-probe test checks all 57 nets for opens and shorts; ask for the report, or check key nets with a meter (at least power, ground and the main buses).
- Look under a lens at the pads, mask registration, silkscreen and edges; check that finish is bright and flat.
- Fit a part (a connector, an IC) on the pads to check the footprint before assembling the lot (see Design Workflow: Schematic to Board).
- Count the boards and keep the package slip: you need it for claims.
- Store them dry in the bag with desiccant if not used within a few weeks (OSP and HASL oxidize).
When the boards are wrong
If a board is not what the files specified (wrong size, missing holes, open nets), photograph it, compare it with the Gerbers, and contact the service within the claim period (often 30 days). A fault caused by the design (a footprint error) is your cost; a fault against the files (a layer missing) is theirs. A viewer-checked file set and a record of the preview you approved make a claim simple.
Troubleshooting
| Symptom | Likely cause | What to do |
|---|---|---|
| Preview shows a wrong or missing layer | Wrong file names or export settings | Rename per the service’s guide; re-export |
| Service queries a design rule | Trace, space or hole below their minimum | Edit the design or accept the surcharge |
| Board size is wrong in the quote | Stray copper or text outside the outline; wrong units | Clean the outline layer; check the units |
| Parts do not fit the pads | Footprint error | Order a corrected board; hand-fix this one with wires |
| Boards delayed in customs | Paperwork or tax | Use the service’s duty-paid option; allow extra time |
| Mask covers pads | Wrong mask layer or expansion | Check the mask Gerber in a viewer |
Related
- PCB Prototyping: the overview of this guide.
- Cost, Quantity and Lead Time: the arithmetic of cost and quantity.
- Assembly: Stencils, Reflow and Assembly Services: after the boards arrive.
- Manufacturing Rules, Files and Design Review: the design rules to load.
FAQ
Which PCB service should I use?
For cheap small boards a low-cost prototype house is hard to beat; for fast local delivery or high quality a domestic service; for hobby work a community service. Compare the total price, rules and delivery time.
How many boards should I order?
At least five; ten if the price is nearly the same: the extras cost little and you will need spares.
Why does the service say my files are wrong?
Common causes: a missing or doubled outline, drill file in wrong units, or a layer in the wrong file name. View the files in a separate Gerber viewer to find it.
How long does a board order take?
About two weeks to the door by express: a day to prepare, a day for the engineering check, about four days to make and five to ship.
What do I do if the boards are faulty?
Compare them with the files, photograph the fault and contact the service quickly. A fault in the files is yours; a fault against the files is theirs.
References
- IPC-6012, Qualification and Performance Specification for Rigid Printed Boards; IPC-A-600; IPC-2221B.
- Fabricators’ published capabilities, file guides and quote pages (JLCPCB, PCBWay, OSH Park, Eurocircuits).
- Ucamco, Gerber Layer Format Specification.
Last reviewed: October 2026. Prices and rules in the worked example are an illustrative model, not a quote.