What to send for a PCB assembly quote

You have a finished layout, a deadline, and a request-for-quote form with a single upload box. You zip the project folder and send it. Three days later the reply is a list of questions, not a number, and the clock has been running the whole time.

An assembly quote is not a price lookup. It is a small engineering review of your design package, and the package decides how long that review takes and how many assumptions the assembler has to make. Missing or ambiguous files create questions that should be resolved before production. This note lists what to send, why each item matters, and common ambiguities to check.

The five things every package needs

Fabrication data for the bare board. Gerbers for every copper, mask, paste and silkscreen layer, plus the board outline and the drill files. Send the paste layers even if you are only asking about assembly, because the stencil is cut from them. Assemblers state this plainly. PCBWay’s assembly file requirements list copper, silkscreen and solder paste as the minimum for assembly review, and that is one supplier’s rule, not a universal one, but it is representative. If your tool can write Gerber X2, use it: the format carries a file-function attribute that tells the reader which layer a file is, so nobody has to infer it from a filename. Ucamco’s Gerber job file does the same job for the board as a whole, carrying thickness, finish and stackup in a machine-readable file instead of a note in an email.

A bill of materials with manufacturer part numbers. Not just values. “10k 0402” is a value; a manufacturer name plus manufacturer part number is an orderable part. If the assembler will select parts, provide the electrical and mechanical requirements and agree on who approves substitutions. Include quantity per board, reference designators, and the package. List approved alternates explicitly. Availability can change between a quote and purchasing, so record who must approve a proposed replacement before it is ordered.

A component placement file. Also called a centroid, pick-and-place or XYRS file. It gives each surface-mount part’s reference designator, X and Y position, rotation, and board side. The placement machine program is built from this file. Without this file or equivalent placement data in an accepted exchange format, the assembler may need additional exports or manual preparation. Ask which formats they accept. Gerber X3 puts this data inside the Gerber set itself. Ucamco describes it as adding component information to Gerber data so the assembler can visualize placement, cut the stencil, program the machine, and check procurement from one package. KiCad 9 can export placement data as CSV or as Gerber X3, and it can also export a complete IPC-2581 or ODB++ package that bundles the board, the placement and the BOM together.

An assembly drawing or a rendered top and bottom view. The placement file says where a part goes. The drawing says which way round it goes. Polarity marks on silkscreen get dropped when someone tidies the silk layer, and a labeled assembly drawing provides a useful orientation reference. Cross-check drawings and 3D models against the component datasheets and footprint pin numbering; an incorrect model can repeat the same error.

The quantity and the revision. Say how many boards, and whether that is one build or the first of several. Say which revision you are sending, and send only that one. A package with three folders named final, final2 and final-really is not a package, it is a puzzle.

What each item actually changes

Buyers often ask why the assembler wants so much. The honest answer is that each file closes off a class of error, and the cost of an error scales with when it is found.

What you send	What it decides	If it is missing
Gerbers plus drill	Fabrication and stencil review	Additional data requested
BOM with MPNs	Part selection and availability	Selection and substitution questions
Placement file	Machine program, side, rotation	Additional preparation
Assembly drawing	Polarity and orientation	Orientation ambiguity
Quantity and revision	Panel layout, setup effort	Requote

The two rows that catch people are the BOM and the placement file, because they look complete when they are not.

The mistakes that survive to the line

These sit next to the layout mistakes that only show up at assembly — one is about the files, the other about the board itself, and a clean package doesn’t fix a bad footprint.

Rotation conventions disagree. CAD exports and machine libraries may use different orientation conventions. Resolve the mapping using labeled assembly drawings and component documentation before placement programming. Do not rely on a visually plausible 3D model alone. Check polarity and pin numbering for diodes, polarized capacitors, connectors and integrated circuits.

The placement export omits intended parts. Export filters and footprint attributes can exclude components. Compare the set of reference designators in the export with the parts intended for that assembly operation, excluding DNP positions. A grouped BOM row can contain many designators, so counting rows is not a useful completeness check. Confirm separately how the assembler wants through-hole placements documented.

Non-purchased features are confused with unpopulated components. Fiducials, mounting holes and printed test pads do not necessarily represent purchased parts. Agree on how to exclude or identify those features in the export. Actual component positions intentionally left empty should have an explicit DNP designation for the relevant build variant.

DNP is not stated per variant. If the same board ships in two configurations, say which references are unpopulated in each one. A single BOM with a DNP column beats two BOMs that drift apart.

The paste layer needs review. Check the paste apertures for exposed-pad packages against the component manufacturer’s assembly recommendations. Agree on the final stencil design with the assembler; they may adjust apertures for the stencil and process they will use. A library footprint is a starting point, not evidence that the final stencil is suitable for every build.

Fiducials and panel information are absent. Global fiducials on the board or panel are what the placement machine uses to correct for board position. If you are sending a single board and expecting the assembler to panelize, say so, and say whether the board has a clear edge for rails. If you designed the panel yourself, send the panel Gerbers and the single-board Gerbers, and label them.

Checks before you press upload

• Open the Gerbers in a viewer that is not your CAD tool. Layer stack, outline, drills and paste should all line up.
• Read the placement file in a text editor. The intended reference designators are present, units are stated, and the side column exists.
• Read the BOM as the buyer will. Every purchased part has an orderable identity or agreed selection requirements, and DNP positions are clear.
• Compare the rendered top view to the schematic for every diode, LED, polarized capacitor and connector.
• Confirm the quantity, the revision, and whether you or the assembler is buying the parts.
• Create a clean release folder containing only the intended revision, then zip it; preserve the design history elsewhere.

How we handle it

Send the Gerbers or an agreed equivalent export, the BOM with part numbers, placement data, assembly drawings, quantity and revision. Include any programming, inspection or functional-test requirements so the scope covers the finished assembly, not just soldering. A clear package makes it easier to identify manufacturing questions before purchasing and production begin.