How to prepare Gerber, BOM and pick-and-place files for PCB assembly in India

31 October 2026 · Sonani Electronics Team

A PCB assembly quote is only as good as the three files behind it. The Gerber set describes the bare board. The bill of materials says which part goes on which designator. The pick-and-place file, also called a centroid or CPL file, says where that part sits and how it is rotated. If those three disagree, the board that comes back will not match the board you simulated.

This note is for engineers and small manufacturers in India who are sending a design out for the first time, or who have been asked to "share Gerber, BOM and CPL" and are not sure what a complete pack looks like. We source the parts and deliver the order. Bare boards and assembly are made through our manufacturing partners. You get a single GST invoice, and the quotation you approve has no hidden charges.

If you only need the bare board, read PCB vs PCBA vs SMT stencil and send the Gerber from the PCB fabrication page. If the parts list is the hard part, use BOM best practices and upload the BOM.

What each file is allowed to decide

The Gerber decides copper, mask, paste, silk, outline and drills. It does not decide which part is bought. "100nF 0402" can still be the wrong dielectric or voltage. How to check a substitute is in alternatives for out-of-stock parts.

The pick-and-place file decides location and rotation. It must use the same designators, units and origin as the Gerber and the BOM. Coordinates from an old outline will place parts off the pads.

Send all three from the same revision. If the schematic changes, export again and say the old zip is obsolete. Each pack you send is kept as its own revision. The PCB terms say how a new file is handled.

What to put in the Gerber zip

Export Gerber RS-274X, not a CAD-only project file. Include a drill file. A typical two-layer board needs:

Top and bottom copper
Top and bottom solder mask
Top and bottom silkscreen, if you use silk
Board outline as a closed shape, preferably on its own mechanical layer
Top solder paste, and bottom paste if the bottom is pasted
A plated drill file, plus a non-plated drill file if your software splits them
Inner copper layers, named in order, if the board is more than two layers

Name files so a stranger can tell layers apart (board-gtl, board-gbl, board-gts, board-gtp, board-outline, and the drill). Put a text file in the zip with the revision, the units, and the stack: layers, thickness, copper, finish, and mask colour. How to choose the stack is in choosing PCB specs.

Use millimetres, and do not mix them with an inch centroid. One board per zip unless you have agreed a panel. A panel changes the outline and every coordinate. Say "panel of N" if that is what you sent.

Before you zip, check that the outline is one closed line, copper stays inside it, mask opens on the pads you will solder, and paste exists for every surface-mount pad that will be pasted. A screenshot of the layout is useful as a picture. It cannot be fabricated.

How to write the BOM so it matches the board

One row per part number. Group designators only when they truly share that part and the quantity equals the number of designators. C1 C2 C3 C4 with quantity 4 is fine. C1-C8 with quantity 4 is not, because nobody can see which four are meant.

Minimum columns that let us buy and place without a meeting:

Column	What to put
Designator	C3, R12, U1. One line can list several if the part is identical.
Manufacturer part number	The orderable number, including the suffix that fixes packing or temperature grade if that suffix changes the part.
Value / description	100nF, 10k, 3.3 V regulator. This is a check, not a substitute for the part number.
Package	0402, SOT-23, LQFP-48. Must match the footprint on the PCB.
Quantity per board	How many of this part are on one PCB.
Fitted or DNP	DNP, do not place, or no-fit if it must stay off the board.

Leave the alternate cell blank until you have checked a substitute. "Or equivalent" does not say who approved it. Internal stores codes can sit in their own column, next to the manufacturer part number, not instead of it.

Write the number of boards in the message: "20 boards". Purchase quantity is per board times that number, plus any extra in its own column. See BOM best practices. If you will supply a part yourself, mark the line "customer consigns this" and still give the designator and package.

Pick-and-place: origin, side and rotation

Export the centroid file as CSV or a spreadsheet. Each placed part needs designator, X, Y, rotation in degrees, and side (top or bottom). Include the unit and the origin in the header or in the text file: "millimetres, origin at the lower-left of the board outline".

The origin must be the same point the Gerber uses. If you move the board on the sheet and export only the centroid, every part shifts. A quick check is to compare the board width in the Gerber outline with the spread of X coordinates. Parts should fall inside the outline, not around some other origin from a previous panel.

Rotation is where a first build goes wrong, because zero degrees is not the same in every CAD tool. For diodes, tantalum capacitors, SOT-23 parts and connectors, add a note ("pin 1 toward the top of the board at zero degrees") or expect a question before assembly. Asking is normal. Guessing places a reel backwards.

Bottom-side parts must say bottom. Leave DNP parts out of the centroid file and keep them on the BOM with a DNP flag, or a machine program can still place them. Hand-inserted through-hole parts can stay off the centroid file, but they stay on the BOM.

Three round fiducials on the top, free of mask, help fine-pitch placement. If the board has none, say so. The manufacturing partner will say if they need marks or a rail.

A short check before you send

Gerber, BOM and centroid are from the same revision, exported on the same day.
Every designator on the centroid is on the BOM, and every surface-mount line that is not DNP is on the centroid.
DNP lines are on the BOM and absent from the centroid.
Quantities match the designator lists.
Units are written once, and they match.
Outline is a single board unless you said it is a panel.
Paste layers exist if you want a stencil or assembly.
The text file states layers, thickness, copper, finish, mask colour and board quantity.

Zip the files. A name like project-revC-gerber-bom-cpl.zip is enough. Send that zip on the instant quote page or on WhatsApp. If some parts are imported and some are from India, the quotation will show the timing of each line. Imported parts typically reach Surat in about 12-15 working days, India-sourced parts about 2-4 working days, depending on stock. After that, dispatch follows the shipping and returns note. The price you approve is the price on a single GST invoice, with no hidden charges.

Common questions

Can I send the CAD project instead of Gerber?

Send Gerber and drill. A native project depends on libraries we may not have. A schematic PDF is welcome and is not a substitute for the Gerber.

Should I hand-edit pick-and-place rotation?

Only if you know that tool's zero point. Otherwise name a reference part (diode cathode toward the connector) and we will confirm with the manufacturing partner before placement.

Do I need the paste layer for a bare PCB?

Paste is optional for a bare board. Include it if you may order a stencil or assembly later, from this same revision. Board, stencil and assembly are different orders: PCB vs PCBA vs SMT stencil.

What if a BOM line is out of stock?

Keep the original part number and add any alternate you have already checked. Package, pinout, voltage and dielectric still have to match. See how to find alternatives, or search parts.