Gerber X2 vs ODB++ vs IPC-2581: what your fab actually wants
Gerber still gets built everywhere, but a plain RS-274X plot carries no nets, no stackup and no component data. The CAM engineer rebuilds all of it by hand, and that is where an open or short gets introduced. X2, ODB++ and IPC-2581 exist to remove that step. Here is what each one carries and when the extra format earns its keep.
What each format carries
Three formats, three levels of intelligence
RS-274X is artwork. A Gerber layer is flashes, draws and regions: geometry with no idea which shape is a pad, which net it belongs to or what the layer is for. The drill file is separate. The stackup lives in an e-mail. The netlist, if the fab wants one, is an IPC-D-356 file somebody has to generate.
Gerber X2 adds attributes on top of that geometry. A pad can be tagged as a component pad with a reference designator and pin number; a layer can declare its function; a net can be named. The fab's CAM tool reads those attributes instead of inferring them from filenames.
ODB++ and IPC-2581 go further and ship a database rather than a picture: stackup, nets, drill spans, component placement and BOM links in one archive. ODB++ is Siemens' format and the de facto input for automated CAM analysis. IPC-2581 is the open XML equivalent, backed by a consortium and accepted by most large fabricators.
| Format | Data model | What it saves your fab | What to check |
|---|---|---|---|
| Gerber X2 | Artwork plus object attributes | Layer identification, pad and net attribution, drill classes | Attributes do not replace a netlist; send IPC-D-356 for net comparison |
| ODB++ (v8.1+) | Hierarchical CAD/CAM archive | Automated net, stackup and assembly checks with no manual rebuild | Proprietary to Siemens; confirm the fab's CAM importer version |
| IPC-2581 | Single open-standard XML file | Design, stackup, drill and assembly data in one non-proprietary file | Support is broad but not universal; confirm the CAM revision |
| RS-274X + Excellon | Legacy artwork and drill | Nothing beyond geometry; works on any tool ever made | Every connection check is manual — the highest-risk option |
Handoff practice
What we send, and why Gerber is still in the box
Every engagement releases a Gerber X2 set as the primary fabrication output. That is deliberate: it is the only format every board shop on earth can open, and a board that cannot be built is not delivered. ODB++ and IPC-2581 go out with it for fabs and assemblers that can use them.
The fabrication notes matter as much as the data. Stackup with dielectric thickness and material, impedance targets and the layers they apply to, surface finish, via classes and any backdrill depths belong in a document the CAM engineer reads before the first tool path. A Gerber set with no notes is a quiz.
- Gerber X2, one file per layer, with the layer function declared in the attributes
- Excellon drill file split by via and component-hole classes
- ODB++ or IPC-2581 where the fab accepts it
- Fabrication notes: stackup, materials, finish, impedance, backdrill, tolerances
- IPC-D-356 netlist when the fab runs an independent net comparison
- Pick-and-place centroid file and BOM for the assembly house
The release package and its verification steps are part of every high-speed PCB layout service and backplane engagement; the format list is identical across services.
Failure modes
The four handoff errors that cost a build
Most fabrication holds are not exotic. They come from a small set of mistakes that survive DRC because DRC only checks the design, not the transfer.
- Units and zero suppression: an Excellon file read as inches when it was written in millimetres puts every hole in the wrong place.
- Mirrored or unnamed layers: a bottom-copper layer without an X2 attribute gets imported as something else and the board is built backwards.
- Stale drill data: vias changed after the drill file was plotted, so the copper and the holes disagree by one revision.
- Missing solder-mask or paste layers: the fab guesses, or the stencil is cut without apertures for the fine-pitch parts.
All four are caught by reading the release package back into a fresh CAM session before it is sent. That read-back is a step in the release, not a courtesy.
FAQ
Common questions
Want this worked through on your board?
Send the stackup and interface list and we will check the fabrication package against a real layout — before the quote is fixed, not after.