-
Notifications
You must be signed in to change notification settings - Fork 1
/
instructions.txt
131 lines (117 loc) · 5.57 KB
/
instructions.txt
1
2
3
4
5
6
7
8
9
10
11
12
13
14
15
16
17
18
19
20
21
22
23
24
25
26
27
28
29
30
31
32
33
34
35
36
37
38
39
40
41
42
43
44
45
46
47
48
49
50
51
52
53
54
55
56
57
58
59
60
61
62
63
64
65
66
67
68
69
70
71
72
73
74
75
76
77
78
79
80
81
82
83
84
85
86
87
88
89
90
91
92
93
94
95
96
97
98
99
100
101
102
103
104
105
106
107
108
109
110
111
112
113
114
115
116
117
118
119
120
121
122
123
124
125
126
127
128
129
130
131
Materials used:
Laser printer with very good toner coverage (fresh toner, toner density set to max)
Cupric Chloride etchant ( https://www.youtube.com/watch?v=V8mHiFYmlBc ) or any other PCB etchant
PCB fab in a box starter kit ( https://pcbfx.com/main_site/pages/products/starter_kit.html )
0.1 or 0.15mm copper film (for stencils, make sure it's actually copper not copper-coated Al. Art supply stores sell it)
Aoyue W002 lead-free solder paste
Solder paste spreading tool (thin metal or plastic strip)
Tweezers
Sponges (dishwashing sponge, use rough side for scrubbing copper, soft side for etching)
Nitrile gloves (lots!)
Isopropyl alcohol for cleaning all the things
Acetone for dissolving toner
Tin-plating solution (we used https://www.buerklin.com/en/tin-powder-for-solder-baths/p/13l217 )
Lots and lots and lots of paper towels
Small polypropylene(!!!) containers for tin plating bath, etchant, and water
Laminator hacked for higher temp operation
Big trash bag
For rework:
Soldering iron
Flux
Really thin desoldering braid
Really thin solder
BOM for board:
4x 27R resistors, 0603, 1%
3x 330R resistors, 0603, 1%
1x 0.1u cer cap, 0603, 50V
2x 22u cer cap, 1206, 25V
2x 47p cer cap, 0603, 50V
1x USB connector, ZX62-AB-5PA(31)
1x ESP-WROOM-32 module
1x 01x10 pin header, SMD, like M20-8771042 or NREC010SABC-M30RC
1x FT231XS
8x RGB LED, ASMB-MTB0-0A3A2
2x push buttons, FSM2JMTR
1x voltage regulator, LD1117AS33TR
Instructions:
Install kicad 4.0.7
Copy template folder to new folder with your own name
Open project file with kicad (ignore any missing library warnings)
Open eeschema
Run ERC
Run CvPcb, make sure all items have an associated footprint, look at footprint if you like
Generate netlist (click net, click generate, click save)
Click on pcbnew button, say yes to create a board
Import netlist
Click view-> switch canvas to default
Click footprint mode button
Right-click, global spread and place, spread out all footprints
View -> switch canvas to opengl
Rotate (R) esp32 and connector right way round
Move (M) RGB LEDs to bottom in correct order and rotate (R) with pin1 top-right
Disabling render/text front might help with seeing things more clearly
To help align the LEDs, use a custom grid - dimensions-grid-millimeters, 7x7 (for example)
Switch grid to user grid, then move LEDs so they align on grid.
Switch grid back to 0.25mm to continue
Move USB port to right side of board
Pin header to left side of board
Two buttons close to their pins
Big caps near voltage regulator
0.1u cap next to ESP32 supply pins
Try to arrange things for minimum crossing lines
Design rules: Default clearance 0.25 default track width 0.3
Design rules: global design rules, custom track sizes 0.4 and 0.6
Dimensions, pad mask clearance, paste clearance -0.1mm
Place parts, and then we start working in exciting mode (X)
Press X, then E
Make sure shove mode is selected, allow DRC violation is not selected
Click on one end of a trace, then move it to its goal
ESC to exit exciting mode, X to reenter it
ctrl-z for undo, u and i for select segment, del for delete
For the power traces use 0.6mm
Add keepout areas to ESP32 module (F.Cu, no copper pour)
-antenna region
-below gnd trace
Add copper pour around board (grid 1mm)
Select layer edge.cuts
Draw board outline
Select layer F.Cu
Draw your name, 2.5mm tall, 2.5mm wide letters using text tool
Hit B to redraw zones
Save!
Use 3D viewer to admire your board
Rendering for etching:
for board: plot, format: ps
disable all layers, enable f.cu
disable all options, enable MIRRORED plot, force A4 output
plot
for stencil: plot, format: ps
disable all layers, enable f.paste
disable all options, enable Exclude PCB edge layer, NEGATIVE plot, force A4 output
plot
For PCB:
Open printer tray, make mark in corner of paper, close tray
Print f.cu file
Cut piece of transfer paper slightly bigger than your design, tape (using paper tape) onto paper so it covers the design and the tape is outside the design area
Insert same sheet of paper into printer in exact same orientation (mark in same corner)
Print again, settings: black and white print, high resolution, paper type heavy
Cut out the design from the transfer paper
Cut piece of PCB slightly bigger than the design
Carefully scrub and degrease the PCB surface (use gloves from now on)
Place transfer paper on PCB surface and run through HOT laminator a few times (2 times is enough with hacked laminator)
Drop in water WHILE STILL HOT
After a few minutes paper will separate, slide it off sideways
Dry PCB COMPLETELY
Place toner reactive film on COMPLETELY DRY PCB so it overlaps one edge, dull side to copper
Run through laminator (one below hottest for modified, hottest for unmodified laminator) once
As it goes into laminator, pull the green film tight to avoid creasing
Allow to cool completely, then peel back film
Etch by dipping sponge into etchant then stroking the PCB with sponge until done
When done etching, wipe everything with paper, then clean with alcohol, then clean with acetone
When done cleaning, scrub copper surface a bit with rough side of sponge, then dip in tin plating solution and leave for a while
Repeat same process for stencil, except:
After green film is applied, tape the back of the stencil and the exposed copper areas around the design in the front
When you are done etching the stencil, the PCB will be ready.
To clean PCB that was in tin plating solution:
Gently take it out, then dry it ENTIRELY with a towel, dip in cold water, dry ENTIRELY again, then wash it carefully under WARM water. Once dry, you can apply paste using the stencil.
Be careful to not overheat during reflow - these boards are thin and the epoxy will delaminate above 270C.