Public:Layout Standards

See ((Schematic Conventions)) for related information about developing your schematic properly before you venture to the layout.

We are developing these standards to increase reliability and professionalism of our team's board designs.

{REMARKSBOX(type="note" title="Note for KiCad 5")}The latest versions of KiCad include a few differences in settings from the older versions. Since we are all using the latest version, please be aware there may be settings you can't find and update these instructions as you find any changes in the software.{REMARKSBOX}

{REMARKSBOX(type="note" title="Units")}Millimeters are fantastic and we encourage using metric dimensions whenever possible, however BAC's standards are written in mils (1/1000 inch) or inches so we present all minimum and recommended dimensions in both mm and mil.{REMARKSBOX}

General

• Traces shall never create 90-degree angle except where absolutely necessary
• Components will always be placed horizontally or vertically, never at an angle
• Space is set aside on boards to provide information about the board
• *Board name
• *Version
• *Blank box for serial number
• *ISC logo
• Component values (e.g. R=100ohms, C=20uF) can be on fabrication layer (doesn't need to be on the silkscreen)
• *When soldering, simply reference a schematic/((Kicad BOM|BOM))
• Put the reference designator (RefDes) on top of the component lengthwise: 300px *Component Placement
• *Top Side
• **Oftentimes components are ideally all placed on the top layer. This is to make soldering easier, although this is somewhat mitigated when there are through-hole (TH) components. Furthermore, after installation signals are easier to probe if they are on the same side, since the bottom is often covered or the chip secured.
• *Both
• **If space is a concern, placing components on both sides is a viable solution.
• **Place replaceable components such as fuses on the top
• **Place indicating components such as lights on the top
• Copper Pour
• *Copper pour minimum width of 0.1mm is too small, increase it to at least 0.2mm
• **0.254mm is a good choice, as it converts to 0.01inches
• Pad mask
• *If possible, decrease pad mask clearance so there is solder mask between all SMD pads of the same chip.

Recommended Dimensions

These are some dimensions you can enter into KiCad when defining clearances and stuff. They have been selected based on Bay Area Circuit's (BAC's) standard design capabilities, which are similar to that of other fab houses. To use the industry terminology, they're dimensions for Low Density Interconnect (LDI) technology PCBs.

Traces and Vias

Traces are the wires of the PCB. They connect components to other components and sometimes to zones (copper pours). KiCad also calls them "tracks". Vias are very small drilled holes in the PCB that are coated with (usually) copper. They connect traces or zones on one layer to traces or zones on another layer. In our designs we recommend not having any blind or buried vias, meaning they connect to inner layers and do not go to one or both outside layers of a board. This goes along with our recommendation of only 2 layer boards if at all possible, so there are only two outside layers.

These dimensions can be set in the Setup -> Design Rules... dialog box. Below are the recommended values for the default net class, and you will likely want to increase them for traces that will carry considerable amounts of current. Don't worry about the settings for microvias (µvias), which we don't use at ISC since they cost extra money to fabricate.

{DIV(clear="both" align="left" width="400px")}

||Dimension|mil|mm

Clearance Min|6 mil|0.1524mm

Track Width Min|6 mil|0.1524mm

Track Width Rec.|8 mil|0.2032mm

Via Dia|27.55901575 mil|0.7mm

Via Drill|11.81098425 mil|0.3mm||{DIV}

These values are suggested minimum values, and can be increased. Feel free to round numbers up. When increasing the via drill size, it is important to increase the via diameter as well, because the difference between the two must be greater than 10 mil (0.254mm) to meet BAC's 5 mil (0.127mm) minimum annular ring requirement. The picture below illustrates what the different dimensions mean.

70px Here is a screenshot of part of the dialog box with the dimensions set. To edit them for your project, simply click on a cell in the table and start typing the new dimension. You are free to double click and copy-paste dimensions from one cell to another. The Net Class function is helpful when you have a number of nets that need the same properties different from the minimums, such as nets at 12V that may carry up to 1A (also make sure your ground "return" paths can handle the same). You can add a new class by clicking the Add button. Give it a meaningful name. To add nets to the class, you must change the dropdown menus under Net Class Membership to be different classes, one the class you're moving nets from and the other you're moving nets to. Select the net whose class you wish to change and click the >>> or <<< buttons to move it to the other class as 70px

Copper Pours

Also known as copper planes, zones (used in KiCad), or a ground plane, copper pours can greatly ease PCB layout and increase PCB performance. These values are set for each copper pour separately, although you can use the "export setting to other zones" button to change the settings of all other pours to match.

• Clearance: 0.2mm
• Minimum Width: 0.2mm
• Antipad Clearance: 0.2mm
• Spoke Width: 0.3mm
• --Segments / 360º: 32-- (does not seem to be an option in KiCad 5)
• Pad Connection: Thermal Relief

These are all minimum values, and they can be increased to meet the needs of your design. It's also worth noting that the settings that dictate how pads connect to pours can be overridden at a footprint level and at a pin level, if you want different pins to connect to the same zone differently.

Pads Mask Clearance

These settings control how the soldermask is spread on your board. Soldermask is the It is important to set them correctly, as soldermask is incredibly useful in making your PCB easy to solder. Soldermask is the green (or some other color) coating on the top and bottom of the PCB. Its purpose is to cover the copper on the PCB to prevent shorts and oxidation, as well as to repell solder so that solder stays where you want it to stay.

• Solder Mask Clearance: 0.1mm
• Solder Mask Min Width: 0.15mm

These values can be reduced slightly if you want to get some soldermask between pins of a tight-pitch IC.

Further Reading

Bay Area Circuits's standard capabilities.