Loading 3D model… large boards can take a moment.
We use KiCad and python script to generate schematic, footprint, and PCB layout with minimal manual intervention.
TMSch.lib. TMSch.lib is symlink-ed to every project. When modifying the library, open the original ```.lib''' file directly instead of opening the symlinks.GenSch.py to generate desired schematic for the TMS array with correct net connectivity. Here we save the generated file as array.sch, which is a 2nd-level hierarchical schematic under Phi10cmBonding.sch.Phi10cmBonding.sch and generate a netlist.KiPcbFp.py to generate a footprint TMS1mm.kicad_mod and save it under TMPcb.pretty which is a footprint library. One may need to modify ~/.config/kicad/fp-lib-table in order for KiCad to find the library: (lib (name Topmetal)(type KiCad)(uri ${KIPRJMOD}/TMPcb.pretty)(options "")(descr "Topmetal bonding footprints")). An alternative is to save a local fp-lib-table file in the project directory.template.kicad_pcb.TMS1mm1chip.{sch,kicad_pcb}. It is preferable to place TMS1mm module's center at the very center in the unit cell. It will be used as a reference (local origin).GenPcb.py which references the netlist-loaded PCB and TMS1mm1chip.pcb, and generates the correctly laid out array.Pull source from https://github.com/KiCad/kicad-source-mirror and compile.
import os, sys, runpy
scriptPath = os.environ['KIPRJMOD'] + "/../KiCadScript"
sys.path.append(scriptPath)
sys.argv = ['', '-h']
fileGlobals = runpy.run_path(scriptPath + "/GenSch2ExDAC.py", run_name="__main__")
cd KiAuto/hexlib/
python setup.py build
cd build
ln -s lib.freebsd-11.0-STABLE-amd64-2.7/hexlib.so .
KiCad schematic sheets are organized hierarchically. Sheet paths are named as /58F9164E/58F91649 with the numbers being timestamps in hex format. Netnames local to a sheet start with a leading /. Global netnames do not have leading /.
| Sunstone preferred | Sunstone capable | |
|---|---|---|
| minimum drill size | 0.008" | 0.005" |
| minimum trace width | 0.004" 1 oz Cu | 0.003" |
| trace clearance | 0.004" 1 oz Cu | 0.003" |
| through-hole pad dia | 0.018" larger than finished hole dia | 0.016" larger |
Finished hole dia = drill dia - 4mil
0.062, 0.093, 0.125, 0.0886(14-layer), 0.0756 (16-layer)
1oz copper thickness is 34um (1.34mil)
0.008, 0.014, 0.020, 0.025, 0.029, 0.033, 0.035, 0.040, 0.043, 0.046, 0.052, 0.061,
0.067, 0.079, 0.088, 0.093, 0.100, 0.110, 0.125, 0.141, 0.150, 0.167, 0.192, 0.251
For boards thicker than 100mil, usually drill size cannot be smaller than board thickness / 10 (aspect ratio).
A recommendation: make the drill size diameter the same as the width of the trace, and the pad size roughly twice the diameter.
width/clearance 6mil/6mil and 4mil/4mil on surface layers, 4mil/7mil and 4mil/10mil inner layers are commonly used for Zo=50Ohm, Zdiff=100Ohm.
No comments yet. Be the first to ask about this board.