A CAM engineer receiving your package has to rebuild the board from files alone: what each layer is, where every hole goes and whether it is plated, how thick the finished board is, and what it must pass. Each file can be syntactically valid and still give a wrong answer: a drill file read in the wrong units, a stale hole list from the previous revision, or a fabrication note that contradicts the purchase order. When that happens, CAM stops and issues an engineering query (EQ), and the job waits for you.
Gerber data preparation is the work of making those answers unambiguous before release. That means knowing which file carries each piece of information, which format settings silently move geometry, which cross-file checks find conflicts before CAM does, how an EQ is properly closed, and where supplier CAM edits stop and design approval begins.
1. What the package must carry, and which file carries it
| Information | Carried by | Common failure |
|---|---|---|
| Copper, mask, legend, paste images | Gerber RS-274X / X2, one file per layer | Layer function guessed from file extension |
| Board outline and cutouts | Profile layer (X2 Profile) or a mechanical layer named in the drawing |
Outline on several layers with different widths; open contour |
| Holes, plated status, slots | Excellon drill files (separate PTH and NPTH), or Gerber drill files | Units or zero format not declared; NPTH merged into PTH |
| Layer order and construction | Stackup drawing; .gbrjob (X2 job file); ODB++/IPC-2581 matrix |
Job file thickness not updated after stackup change |
| Connectivity | IPC-D-356 netlist, or net attributes in X2/ODB++/IPC-2581 | No netlist, so a copper short to a plane cannot be detected against design intent |
| Dimensions, tolerances, finish, class, tests | Fabrication drawing and notes | Drawing at a different revision than the data |
| Revision identity and file list | Release manifest | No manifest, so mixed revisions go unnoticed |
Gerber images describe geometry only. The Ucamco Gerber Layer Format Specification defines X2 attributes that also state what the geometry is:
%TF.FileFunction,Copper,L1,Top*%
%TF.FilePolarity,Positive*%
%TF.SameCoordinates,TRAIN-C-RevC*%
%TA.AperFunction,ViaPad*%
%TO.N,GND*%
FileFunction removes layer guessing. SameCoordinates declares that every file in the set shares one origin. AperFunction separates SMD pads, via pads and conductors, which CAM uses to apply mask and compensation rules. .N attaches nets to objects. The attributes help only if the receiving CAM flow reads them, so confirm that the fabricator imports X2 before relying on them.
Format choice
| Format | Strength | Release check |
|---|---|---|
| Extended Gerber RS-274X | Universal support; files are easy to inspect | Layer function, stackup and nets live in companion files |
Gerber X2 + .gbrjob |
Layer function, pad function and nets in the images; machine-readable job data | Receiver must read the attributes your EDA tool actually writes |
| ODB++ | Single structured product model with layers, drills, nets and components | Version compatibility and import report |
| IPC-2581 (DPMX) | Open standard, bidirectional; can carry stackup and BOM | Agreed revision and content level; import validation |
The Gerber Job format specification defines how the .gbrjob file carries board-level data such as thickness and layer structure. It does not set which document governs when the job file, drawing and purchase order disagree. That has to be agreed per project (Section 5).
Use a format both sides can export, import, compare and archive without losing information. HILPCB accepts Gerber RS-274X/X2 and ODB++ for fabrication and assembly quotes.
2. Drill data: the format errors that move holes
Excellon drill files are plain-text coordinates, and their meaning depends on header settings that some tools omit. Two settings change geometry without any error message:
| Setting | Example | Misread as | Result |
|---|---|---|---|
| Units | X025400 intended as 25.400 mm (3.3 metric) |
2.4 inch | 2.5400 in = 64.516 mm, scaled by 2.54 |
| Zero omission | X254 in 3.3 mm, leading zeros omitted, so 0.254 mm |
Trailing zeros omitted | 254.000 mm, scaled by 1000 |
A scaled drill file usually looks obviously wrong in a viewer. A file whose coordinates fall back on the board by coincidence, such as small offsets on a panel, can pass a quick look. Declare units and number format explicitly in the header (METRIC / INCH, and the digit format), and keep one convention across all drill files. Gerber files avoid this ambiguity: the current Gerber specification requires %MO units and %FS format, with leading-zero omission only.
Three more drill checks:
- PTH and NPTH in separate files. Plated status decides whether a hole is drilled before or after plating and how it is toleranced. A mounting hole merged into the PTH file comes back plated.
- Tool sizes are finished sizes unless stated otherwise. State on the drawing whether the drill table lists finished hole sizes or tool sizes. The fabricator chooses the tool after allowing for plating thickness. See finished hole size and drill tolerance.
- Slots and blind/buried spans. Give routed slots as slot commands or a route layer, not as overlapping hits. Give each blind or buried via span in its own file, named with its start and end layers, and match it to the stackup.
3. Preflight: inspect the export, not the CAD session
Open the final archive in an independent Gerber/CAM viewer. A check inside the EDA tool shows that the design is correct there, not that the export is.
Geometry and images
- Layer count and order match the stackup; all layers share one origin and register over each other.
- The board outline is one closed contour. Cutouts, slots, castellations, edge plating and V-score lines appear on the layer the drawing names.
- Top legend reads correctly from the top. Bottom layers follow the viewing convention stated on the drawing.
- Copper-to-outline clearance is met, including at V-score lines and breakaway tabs.
- Solder-mask openings, mask webs between fine-pitch pads, and tented/plugged/filled vias match the via-treatment note feature by feature.
Cross-file checks
- Drill spans match the stackup for every blind and buried via.
- PTH/NPTH holes land on the pads and mechanical features they belong to.
- The IPC-D-356 netlist matches the copper. A netlist comparison finds a short to a plane or a broken connection that the images alone cannot reveal, because CAM has no other source for design intent.
- Paste layer, BOM, centroid file and assembly drawing agree on reference designators. See the pick-and-place file checklist.
4. The release manifest and what a checksum proves
Put a manifest inside the archive and make it match the purchase order and the drawing title block:
- Product identity: part number, board name, revision, variant.
- Source identity: CAD tool and version, project revision or commit hash.
- File inventory: filename, function, layer, units.
- Integrity: SHA-256 for each file.
- Applicable documents: revision of the fabrication drawing, stackup, impedance table, material specification and assembly requirements.
- Supersession: which earlier package this replaces.
A SHA-256 match proves that the received file is byte-identical to the file listed. It does not prove that the listed file is the right one, that the set is complete, or that the drawing and data agree. A manifest that faithfully hashes a revision B hole list inside a revision C package simply confirms the error. Generate the hashes after the cross-file checks, not before.
5. Conflicts and engineering queries
When two files disagree, CAM should not guess which one is right. It issues an EQ, and the job holds until the design owner answers.
| Conflict | Fabricator's responsibility | Designer's responsibility |
|---|---|---|
| Outline vs. drawing dimension | Stop CAM and issue an EQ; do not scale to fit or pick a datum | Confirm the dimensioned outline, or supply corrected data |
Stackup drawing vs. .gbrjob |
Report the mismatch; do not substitute dielectrics, since impedance changes | Confirm the stackup revision and regenerate the job file |
| Drill file vs. pad geometry | Flag tool-size mismatch or unclear plated status | Supply a corrected hole table with the drill and pad data |
| Mask image vs. via-fill note | Flag it; tenting, plugging, filling and capping are distinct processes | Define via treatment per feature and its acceptance criterion |
| Impedance table vs. routed width | Calculate the width for the real materials and propose a change | Review the solver result and approve the stackup proposal in writing |
| Notes vs. purchase order | Hold and ask which governs | Correct the governing document and record the change |
An EQ is closed when three things exist: a named decision-maker's answer, a replacement file or document that carries the answer, and a scope (this lot only, or all future orders). An email reply with no replacement file closes nothing, and the next order repeats the conflict. Keep the EQ log in the release folder. HILPCB's CAM engineers issue EQs from the DFM review and hold the job until each one is answered.
6. Where CAM edits stop and design approval begins
Every fabricator modifies working data. Separate three kinds of change:
- Routine compensation within the agreed scope. The supplier may prepare compensated working data to achieve the released finished requirements, where the order and CAM permissions allow it. Examples are etch compensation on trace width, drill oversize for plating, and mask opening adjustment within the stated mask-to-pad rule. The finished board must still meet the drawing. Changes outside that scope require the appropriate approval. Calling an edit "compensation" does not authorize a change to design intent.
- Panel and tooling additions outside the board outline. Rails, tooling holes, fiducials, test coupons and copper thieving in the panel border. These are normally agreed with the order. Thieving or balancing copper inside the outline is a design change. See copper thieving.
- Design-intent changes, which need written approval. Changes to annular ring, routing, padstacks, spacing, connectivity, hole types or plated status, the board outline, or the stackup materials. Swapping a dielectric, even for an "equivalent" grade, also needs requalification of impedance and thermal behavior.
Write this boundary into the fabrication notes rather than leaving it to the supplier's default. "Supplier may adjust trace width ±10% to meet impedance; all other copper changes require approval by EQ" is a clear permission. "Supplier may optimize for manufacturing" is not.
7. Worked package: three conflicts in TRAIN-C Rev C
Board TRAIN-C Rev C is released as package CTRL-C-01. Preflight and CAM review find three conflicts:
| EQ | Conflict found | Decision | Replacement evidence | Scope |
|---|---|---|---|---|
| EQ-01 | Drawing says ENIG; purchase order says OSP | ENIG confirmed | po-amendment.txt (APP-01) corrects the order | TRAIN-C only |
| EQ-02 | Revision B hole list inside the revision C set | Revision C hole record governs | hole-list-rev-c.csv (APP-02) replaces it | TRAIN-C only |
| EQ-03 | Job summary says 1.50 mm; stackup says 1.60 mm | 1.60 mm stackup entry governs | Corrected job-summary.json (APP-03) | TRAIN-C only |
Each answer arrives with a file that carries it, so a reader of the next package does not need the email thread. There is no rule that "the drawing always wins". EQ-01 corrected the purchase order, EQ-02 replaced a data file and EQ-03 replaced the job summary. Document authority is a project decision and has to be named.
The new package CTRL-C-02 supersedes CTRL-C-01 and lists every replacement in its manifest with SHA-256 hashes. The fabrication notes and EQ log close the loop.
The package is still not releasable. Closing three conflicts makes the files consistent with each other. It does not make them complete. The manifest status stays HOLD - incomplete fabrication requirements, because actual hole geometry and tolerances, the board-thickness tolerance and the required test reports are still undefined. The job summary carries only board identity, revision and thickness. A complete .gbrjob also carries the layer structure and fabrication characteristics. A package can be internally consistent and still be missing requirements, and CAM will raise EQs for every one of them.
8. Comparing quotations against the same release
Two quotes are comparable only if they answer the same package. Check each one for:
- The package ID and revision it quotes (CTRL-C-02, not "your latest files").
- Exceptions: any changed tolerance, material, finish or test, listed line by line.
- Open EQs assumed answered in the price, and how they were assumed.
- Test scope: electrical test against netlist, impedance coupons, microsection, and which reports are delivered.
- Lead time counted from the point where all EQs are closed, not from file upload.
If engineering accepts a commercial alternative, such as a different finish or material, update the controlled documents so the next order does not repeat the same EQ.
9. What to send for a fabrication quote
- Gerber X2 or RS-274X (or ODB++/IPC-2581), with a profile layer and one file per layer.
- Excellon drill files, PTH and NPTH separate, with units and number format declared, plus span files for blind/buried vias.
- IPC-D-356 netlist.
- Fabrication drawing: stackup with finished dielectric thicknesses, impedance table, finish, mask and legend colors, via treatment per feature, tolerances, IPC class and revision, test and report requirements.
- Release manifest with SHA-256 hashes and supersession note.
- CAM permission statement (Section 6).
For drawing content, see fabrication drawing essentials. For panel requirements, see the panelization design guide.
HILPCB's CAM engineering team reviews every multilayer PCB and HDI PCB package before tooling. The review covers layer and drill import, netlist comparison, stackup and impedance, and via treatment. Questions go back as EQs, and compensation stays inside the permissions stated on your drawing. For HDI quotes, a DFM and pricing analysis is typically returned within 2 hours of a complete package. Upload your release archive to request a quote.
Frequently Asked Questions
My drill file opens in the viewer and the holes look right. Can units still be wrong?
Yes, if the viewer guessed the format. Many viewers auto-detect units and zero omission when the header is missing. The fabricator's CAM may guess differently, or may stop and ask. Check that the Excellon header declares units and number format, and that the viewer reports it read them from the file rather than from a default.
Is an IPC-D-356 netlist still needed if I send Gerber X2 with net attributes?
Only if the fabricator's electrical-test flow reads X2 net attributes. Many test fixtures and flying-probe programs still take the netlist from an IPC-D-356 file. If no design netlist is supplied, the fabricator can only extract connectivity from your copper, so a short in the copper is tested as intended. Send the netlist unless the fabricator confirms another source.
Can the fabricator change trace widths to hit my impedance target?
Only within the permission you state. The fabricator can propose widths calculated for its real materials and pressed thickness. Without a written permission such as "±10% width adjustment allowed for impedance", any width change is a design-intent change that needs EQ approval. State the permission on the drawing so the job is not held waiting for an answer.
If every file in my manifest matches its SHA-256 hash, is the package correct?
No. A hash proves the received bytes match the listed file. It cannot show that you listed the right revision, that a required file is missing, or that the drawing and data agree. Run the cross-file checks first, then generate hashes for the files you have actually checked.
