mirror of
https://github.com/skogaby/KFChickenShim.git
synced 2026-09-10 03:25:18 -05:00
196 lines
4.1 KiB
Markdown
196 lines
4.1 KiB
Markdown
## SFE Process for Board Design
|
|
|
|
### Prepare
|
|
|
|
Prerequisites:
|
|
|
|
* This repo is up-to-date
|
|
* SFE default settings are applied
|
|
|
|
Make a new project and save it to working /hardware directory.
|
|
|
|
### Schematic
|
|
|
|
Open the eeschema
|
|
|
|
Setup the frame:
|
|
* File -> Page Settings
|
|
* Import date (click <<<)
|
|
* Enter version number "v01"
|
|
* Enter board name
|
|
* Enter company name "SparkFun Electronics"
|
|
|
|
Set up the libraries
|
|
* Preferences -> Component Libraries
|
|
* Remove all
|
|
* Add all .lib files from this repo
|
|
|
|
**Draw schematic** - for this make LM1117 LDO circuit with two pin input, two pin output, input cap, output cap
|
|
|
|
#### Place symbols
|
|
|
|
Hotkeys
|
|
|
|
* '?' show hotkeys
|
|
* 'a' to add component
|
|
* 'p' to add power symbol
|
|
* 'r' to rotate
|
|
* 'x' and 'y' to mirror
|
|
* 'm' to pick up
|
|
* 'g' to drag (keeping wires)
|
|
|
|
Components
|
|
|
|
* 10UF 16V on input
|
|
* 10UF 6.3V on output
|
|
* LM1117
|
|
* 240 ohm resistor on high side
|
|
* 105 ohm to ground
|
|
* 2 2-position 0.1 inch headers
|
|
* Gnd from power symbols
|
|
|
|
#### Draw Nets
|
|
|
|
**Consolidate parts**
|
|
|
|
* Use 'g' to drag, 'm' to move.
|
|
|
|
**Clean up labels**
|
|
|
|
* Use 'm' over text
|
|
* Use 'e' to shorten text
|
|
* Orient PROD-IDs similarly and move to readable location (In this example, vertical text placed above works well)
|
|
|
|
**Name nets**
|
|
|
|
* Use 'l' to add label, use 1mm size, make sure point is attached to net (no floating labels)
|
|
|
|
This design has 4 nets:
|
|
* PWR_IN
|
|
* PWR_OUT
|
|
* FB
|
|
* GND
|
|
|
|
#### Prep for Layout
|
|
|
|
**Annotate symbols** -- Use annotate symbol button
|
|
|
|
**Associate components**
|
|
|
|
The first time this is run, no footprints exist. Click through the dialogs. Then go Preferences -> Footprint Libraries, click "Append with Wizard", group select all .pretty folders from this repo, and add.
|
|
|
|
Close the associate dialog and re-do now for auto part search
|
|
|
|
Select a footprint in the right-hand pane for each part.
|
|
|
|
Save the association, then close the dialog
|
|
|
|
Click "NET" button to generate a netlist, and save.
|
|
|
|
Save and close the schematic.
|
|
|
|
#### Setup Pcbnew
|
|
|
|
**Configure frame** - Use File -> Page Settings as in eeschema
|
|
|
|
**Import netlist**
|
|
|
|
Open Pcbnew
|
|
|
|
Use "Read Netlist button"
|
|
|
|
Click "Read Current Netlist"
|
|
|
|
Now you have a pile of parts in your frame.
|
|
|
|
**Build net class matrix**
|
|
|
|
Select Inches in left toolbar.
|
|
|
|
Open Design Rules -> Design Rules
|
|
|
|
Add two new classes:
|
|
|
|
* Bulk - 10 mils clearance, 16 mils width, 15 mils vias drill, 24 mils via size
|
|
* Signal - 8 mils clearance, 8 mils width, 15 mils vias drill, 24 mils via size
|
|
|
|
Assign nets:
|
|
|
|
* Add PWR_IN, PWR_OUT, and GND to bulk membership
|
|
* Add FB to signal membership
|
|
|
|
#### Perform layout
|
|
|
|
View must be set to default to organize parts. Use menu or press F9.
|
|
|
|
Click IC with arrows (Mode: footprint)
|
|
|
|
Right click on component pile -> global spread and place -> spread out all footprints
|
|
|
|
**Arrange components**
|
|
|
|
Switch to opengl view (F12)
|
|
|
|
**Route Tracks**
|
|
|
|
Click on "Add tracks and vias" (Right bar)
|
|
|
|
"d" becomes drag track/via
|
|
|
|
**Add board edges**
|
|
|
|
Set grid to 50 mils
|
|
|
|
Set layer to "Edge cuts"
|
|
|
|
Select graphic line tool (Right bar)
|
|
|
|
Draw edges
|
|
|
|
**Add ground pours**
|
|
|
|
Select F.Cu layer
|
|
|
|
Select "Add filled regions" (Right bar)
|
|
|
|
Start drawing, will generate edit dialog
|
|
|
|
Select GND
|
|
|
|
Set min width, clearance
|
|
|
|
Finish drawing
|
|
|
|
Repeat on B.Cu
|
|
|
|
Save design
|
|
|
|
**Clean up board**
|
|
|
|
Press alt-3 - There's a bunch of excess text.
|
|
|
|
Hide unwanted text with 'e'
|
|
|
|
Some designs want designatiors on the silk for reference, if so move them where you like.
|
|
|
|
View hidden text through render tab in right bar.
|
|
|
|
**Go back and add a SparkFun logo**
|
|
|
|
Save the design, close it, go back and open eeschema. Add a SFE flame and OSH logo above the info box. These are components so associate them, generate a netlist, and open that netlist back in pcbnew. Then, arrange the silks. Add some text too if you like, try 0.03x0.03 size.
|
|
|
|
**Add standoffs**
|
|
|
|
Just like the logos, standoffs have a symbol and footprint.
|
|
|
|
**Add stitching vias and fiducials**
|
|
|
|
From pcbnew, add a footprint directly ('o').
|
|
|
|
Vias are located in hardware. Name it the correct net, hide the text, then copy.
|
|
|
|
Fiducials are located in aesthetics.
|
|
|
|
For both, select the zone frame and re-select fill to have it recalculate zone clearance.
|
|
|