If you hide footprint values, are they reflected into Gerber files when you plot? Also, how can we make visible the hidden footprint values after plotting gerber files

Yes and no. The Gerber file unequivocally reveals whether two points are connected. Only the geometry is needed. If you know the locations of the net endpoints, you know the net. However, do you know the end points? You can make a good guess from the traces, but it is far from perfect. Consider pads embedded in copper pours, etched components, non connector copper such as text and logo’s. Non-connected pads still need to be isolated from other nets. A trace can connect to a copper pour, which is not an endpoint. From the geometry you can make a guess at the netlist, but it is not reliable.

Remarkably, most fabrication data sets do not contain an explicit netlist, but the fabricator is expected to do an electrical test. That is paramount to telling the fabricator: “You must test the netlist, but what the netlist is, you guess.” It is one of the mysteries of this industry that this is the established workflow. With an explicit netlist, there is no need for guessing.

Adding the netlist has another advantage. If there is any error in the output or input of the Gerber files, chances are that it will change the netlist. The fabricator can check whether the geometry fits the netlist. Thus adding the netlist is a very powerful checksum on the image. I consider it completely daft that this is not used routinely.

1 Like

Over the years manufacturers have become quite good at guessing pads in gerbers, but in the older versions the concept of a “pad” did not even exist. It’s just flash codes at some locations. (flash codes are like postage stamps. you stamp the form of it somewhere on the PCB. Even if a pad is not visible (in a zone, no thermal relief) the flashcode may still be there, and also on the solder mask layer.

In newer Gerber revisions X2 or X3, the full netlist and all pad locations can be embedded and this removes the need for guesswork, and makes automation easier. One use for this is flying probe tests. But this needs pad locations, and not the BOM.

One use of the BOM could be to check for mismatches between the parts and footprints.

If you’re interested about gerber details, the Gerber format is maintained by Ucamco (a manufacturer of gerber plotters) and the standards are freely available.

Currently KiCad also only supports a sub-set. the newest (X2 or X3) version for example specifies a specific layer for V-grooving and it has features for defining “copper items” such as PCB inductors and closed solder jumpers, so more guesswork can be eliminated for things such as flying probe tests.

True, fabricators are good at guessing the netlist. They have to. But it is guessing. As so often in this industry, we do not solve the root problem, but live with the problem, and organize ourselves around it.

Also true, with X2 the pads can be identified unequivocally, and then the netlist can be determined from the geometry, without guessing. But the netlist is still a powerful checksum, one wonders that it is not included more often. Note that this is regional, the vast majority of US datasets contain the netlist. Not in Europe - a self-inflicted competitive disadvantage.

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.