PCB component layer names

[vanepp]

Documentation is unfortunately lacking. Someone capable of and willing to write documentation is highly desired, we just haven’t found someone yet . Here are two tutorials that apply to the current version of Fritzing (most others are for older versions of Fritzing):

Fritzing PART CREATION Video Tutorial Series

Fritzing Part Creation - Chapter3 - Inkscape Advanced Essentials Learning how to draw in Inkscape - more features. 0:00 Overview 0:16 Select object with cursor and XML Editor 3:34 Manipulate special PDF’s in Inkscape 4:33 XML Editor - Direct drawing manipulation 6:05 XML Editor - Making group, moving object, changing layer height 7:27 Cursor - Changing layer height 8:21 Ruler 9:07 Grids 9:28 Snap selection 10:16 Drawing origin

Part creation howto part 1 breadboard and pcb

Someone in this forum post requested help to fix up a part. So while doing that I decided to record what I needed to do in order to fix the part to provide a tutorial to create new / fix broken parts. If you start from the Tarjeta S4A EDU.fzpz file posted in the above thread, you should be able to recreate my improved part posted in the same thread. I started by loading the original part in to Fritzing, that indicates breadboard is (at first look anyway) pretty good, but schematic and pcb are…

If you find parts that are unclear in mine, feel free to post and I will try and fix them up, Old_Grey hasn’t posted in a while and I think may have moved to Kicad as the project he is involved in what moving that way. Now for direct answers to your questions (I also use Inkscape):

pcb wants by default (it is actually specified in the fzp file for the part in the layers section) these groups in this order:

Through hole part:

group silkscreen
silkscreen drawing elements
group copper1
group copper0 (this is a subgroup of copper1
copper drawing elements (usually a circle for a connector pin, but sometimes something like a path for an oblong connector). There are other fields available but these 3 are the common ones. A SMD part omits the copper0 layer so has only silkscreen and copper1.

@leopard

but only then allows connections to the centre of the component

As far as I know this is the only way connections will be made in pcb.

@leopard

and can’t find how to define drill holes

In Inkscape a hole is created by a circle with a stroke-width of 20thou (which depends on drawing scale). The hole size = circle-diameter - (2 * stroke-width), so for a .1 header (where the hole wants to be 0.038in, the diameter of the circle wants to be 0.078in with a 20thou stroke width that creates a 0.038 hole in the gerber output. You can also do this with a circular path (but only a circular path, oblong doesn’t work as far as I can tell), but a circle is preferred because it is easier to change later. Oblong pads as you want are created by overlaying a oblong path over a circle (whose id is connectorxpin where the path is unnamed both in copper0 as SMD doesn’t drill holes.) I can point you at parts with oblong pads if you like, often copying an existing part is the easiest way to make parts.

@leopard

also is there a standard set of colours for stuff like silk screen items.

Yes, they are defined in the graphics standards here:

http://fritzing.org/fritzings-graphic-standards/

the part file format is also a very useful document:

2.1 Part file format

All of that said, the usual way (and the way I learned to make parts) is to ask questions here, preferably uploading the .fzpz file of the part you are making so one of us can look it over and tell you what is wrong. Upload is 7th icon from the left on the reply menu.

Peter