Getting a Through Holes Board Produced


I have just completed a layout for a board (it is my first), and I am preparing to send it off to get shipped, but I am worried about the layers.

So far, all I have used is the top and bottom copper layers, the edge.cuts layer, and the silkscreen layers. A default kicad project has a bunch of other layers (adhesive, silkscreen, soldermask, eco1/eco2, cmts, dwg) what are these layers used for and do I need to worry about putting stuff on them if my project is nothing but through-holes?

Hereis the link to my project page.
Also, is anyone is willing to (and is it ok to ask here) give it a once over as well and see if there are any other issues? I am planning to order it through Oshpark because they are pretty cheap.


For manufacturing you also need the soldermask layers.

And the drill files, plated and non-plated (if you have non-plated holes).


What about the soldermask? Do I need to add something to that layer, and I assume drill files is part of the gerber export? I am really fresh at PCB Design, and trying my hand at it.



What goes on the soldermask layer? I know the soldermask is the coating on top of the copper, but what do I put there? I thought the entire board already has an automatic soldermask.


If you don’t include the soldermask gerber file, then the board house won’t put a soldermask on your board.


Your fabricator (Oshpark) almost certainly has instructions on their web site regarding the files they require and some details about generating the gerber files. They may prefer a file-naming convention that uses the filename extension to indicate the file’s purpose (e.g., ".TOP for top copper, “*.BSM” for bottom solder mask, etc.). There are slight variations from one vendor to another, so be sure to read their instructions.

They definitely need top and bottom copper layers. They may have specific instructions about the data format within the gerber files (e.g., “4.5” versus “4.6” precision, imperial versus metric, etc). In many cases they will tolerate any current data format supported by Gerber, but they probably have one format that is preferred. They almost certainly want the “RS-274X” file format, NOT “RS-274D”.

They also need drill information, in Excellon format. Creating separate drill files for the plated holes, and unplated holes, is the most customary practice but some fabs may ask for a combined file. Ecellon also has options for data representation - ask the fabricator which they prefer.

A few fabs will produce “naked boards” - just copper layers; no silkscreen; no soldermask - at cheap prices and quick turnaround but usually we get soldermask (both top and bottom) and silkscreen. The long-running “standard” is silkscreen on top only but a few places will do silkscreen on both sides at no additional charge.

Pay attention to how they want the outline treated. Some ask for a separate outline (“EDGE.CUTS”) layer with absolutely NOTHING else on it; others will ask for the outline to show on EVERY layer; a few may ask for an outline included on a particular layer.

In the “good old days” (formerly known as “these difficult times”) the fabricator liked to have a dimensioned drawing of the board outline, perhaps showing locations of significant holes (e.g., mounting holes). I produce this (along with all the fabrication notes) on the “.DWGS.USER" layer; others use ".CMTS.USER” or one of the “*.FAB” layers.

Don’t include additional layers if they are not used - that creates an environment where confusion grows. The paste layers are used to make solder-paste stencils for assembling surface-mount boards. The adhesive layers are for placing glue that holds components into place during assembly (absolutely critical for SMT parts located on the bottom side of a two-sided board!). “CRTYD” layers are mostly to guide component placement during layout, to ensure there is enough “elbow room” around parts during assembly. Some users create assembly drawings in the “*.FAB” layers; others use them to send information to the raw board fabricator (much like I use DWGS.USER). “CMTS” and “ECO” layers typically have purposes specified by local administrivial processes or the designer’s personal workflow habits.



Or, the job will get placed into a never-never land of “On Hold” while the fabricator finds out whether you really want soldermask or not. That may also happen if your files don’t match the fabricator’s expectations for other reasons.



I think I get it. To sum up, soldermask is where to leave out soldermask and pads already do that automagically, Paste and Adhesive are only needed for SMD parts, The others are either by company request or by user wish.

So all I have to do is double check soldermask, export files, and I am good to go


You probably want the “PLOT” menu in PCBNew, rather than “Export”.

And after you have gerber files, open them in a gerber viewer and spend a little time looking at the individual layers, and combinations of layers. Are the pads, traces, silkscreen, etc, where you want them to be? Did any strange traces creep in when you weren’t watching? Do any of your pads have silkscreen on top of them? Do any vias pop through where you don’t want them to be? Did you allow a setback (at least 10 mils - perhaps as much as 30 or 40 mils - depending on your board house) between the board edge and any copper feature? Are the solder mask openings a few mils larger than the pads?

Many board houses will catch at least some of these errors, and either correct them without telling you, or ask if you really want to do this. Others will build the board, mistakes and all, just like your files describe it.



You probably want the “PLOT” menu in PCBNew, rather than “Export”

I was using export generically.

And after you have gerber files, open them in a gerber viewer and spend a little time looking at the individual layers, and combinations of layers.

Now why did I not think of that? Thanks.


An EDA tool I used previous to KiCAD placed the Gerber-creation process under the “Export” menu. When I came to KiCAD I experienced some frustration while searching the “Export” menu for a way to make Gerbers.

The final review of Gerber files before sending them off to a board house is a step that’s too often neglected. Forcing yourself to look at your work from the perspective of a different tool often uncovers stupid mistakes that were hiding in plain sight. Or, some minor layout task that you intended to do but never got around to it. A typical layout program like KiCAD presents a LOT of visual information in its displays, and the sheer volume of it all means that sometimes things get overlooked. A final review - performed seriously, not just a perfunctory glance so you can mark a check-list - can save a lot of money and personal embarrassment.