Skip to the content
8 layers110 × 69 mmEVO2513, the printed circuit board in 3D

PCB design for the evoone BMS

Size
110 × 69 mm
Copper layers
8
Thickness
1.59 mm
Parts
271
Nets
171
Pads
1,053
Tracks, vias
1,595, 1,474
Pours
500
Routed
Yes
KiCad
KiCad 10.0 (file 20260206)
Created
9 Sep 2026
Updated
6 Nov 2026

Overview

EVO2513 is an open-source printed circuit board by evosonic, from the evosonic/evoone-bms-pcb repository on GitHub. It is an 8-layer board of 110 × 69 mm with 271 parts on 171 nets, routed with 1,595 tracks and 1,474 vias.

It is built around the TLV9002IDSGR, DMT4011LFG and BSS138, with the QTLP600C4TR, B340A and DT1240V3-04LP among its other parts. Its parts include 113 resistors, 58 capacitors, 21 transistors, 10 diodes and 6 connectors. It belongs with the power boards of this library.

Main components

8

README

README.md

EvoOne BMS PCB (EVO2513 v0.6.0)

KiCad project for the EvoOne battery management board, EVO2513 revision 0.6.0. Revision 0.6.0 is the 0.5.0 design (the boards in field test) with the W16 review changes below. The project, schematic and PCB files are named EVO2513; the project libraries keep their EVO2513-0_5_0 names.

The design was converted to KiCad from the Altium sources supplied by Lattech. The raw import needed several fixes before the schematic and PCB agreed; see Fixes after import.

Board

Outline110 × 69 mm
Layers8 copper (F.Cu, In1–In6.Cu, B.Cu)
Thickness1.598 mm finished (1.59 mm laminate + ENIG); stackup as the Altium fab drawing: three 0.25 mm cores, 2116 prepregs, 1 oz copper
Components~230 footprints
ToolKiCad 10.0

Schematic sheets

The schematic is hierarchical: the root sheet EVO2513.kicad_sch holds one sheet symbol per sheet, and each sheet is its own file. Open it from EVO2513.kicad_pro.

SheetFunctionKey parts
S01 External ConnectorsBoard connectors, mounting and test pointsJ1–J6, TP1–TP26
S02 Input ProtectionOver/under-voltage and reverse-voltage protection on the inputLTC4365, DMT4011LFG N-FETs
S03 BMS Input and Output MonitorInput/output current sensing and power-path switchingLTC1960, DMP3018SFV P-FETs, 2512 shunts
S04 Charger RegulationCharger switching stageLTC1960, L1 4.7 µH
S05 Battery ManagementDual-battery selection and managementLTC1960
S06 STEP-Up Step-Down RegBuck-boost output regulatorLM51772, L2 0.68 µH
S07 Load Switch and I-SenseOutput load switches and current-sense amplifiersTPS22811 ×3, TLV9002 ×2
S08 IO ExpanderSPI I/O expander driving the rail enables and reading the faultsPCAL9714

The LTC1960 dual battery charger/selector is a single IC (U1) split across sheets S03–S05.

Nets that cross sheets leave each sheet through a hierarchical label and a pin on its sheet symbol, and the root sheet joins the pins with local labels. There are no global labels; those nets are named from the root (/DCBMS, /POS1, …). Labels between device sheets show the direction of power or signal flow (e.g. DCFILTERED is an output of S02 and an input to S03); links to the connector sheet, S01, stay passive. Labels used on only one sheet are local, and power nets use power symbols.

Connectors

RefPart
J1Molex 1053101204, 2.5 mm pitch
J2Molex 1053101114, 14-way 2.5 mm pitch, vertical
J3Amphenol BergStak 10144517-043802LF, 40-pin 0.8 mm receptacle
J4Molex 1053102204, 2.5 mm pitch
J5, J6Molex 1053091102, 2-way 2.5 mm pitch

The thermistor nets on J3 pins 24 and 28 are deliberately swapped from the Altium design. The swap went in with 6ce5d68, whose commit message doesn't mention it. Firmware written for the earlier pinout must swap its BMSTEMP and REGTEMP channels.

J3 pinAltium designNow
24BMSTEMP (TH1)REGTEMP (TH2)
28REGTEMP (TH2)BMSTEMP (TH1)

Files

  • EVO2513.kicad_pro — project
  • EVO2513.kicad_sch — root schematic sheet; S0x *.kicad_sch — the eight sheets
  • EVO2513.kicad_pcb — PCB layout
  • FIRMWARE_NOTES.md — what the MCU firmware must know about this revision: SPI and expander set-up, the inverted DAQ enable, load-switch thresholds and current-monitor scaling
  • EVO2513-0_5_0-import-fps.pretty/ — project footprint library (footprints extracted by the Altium import), registered in fp-lib-table. Chip resistors and capacitors, the small diodes and the LEDs instead use KiCad's standard libraries (Resistor_SMD, Capacitor_SMD, Diode_SMD, LED_SMD, Package_TO_SOT_SMD, Package_DFN_QFN)
  • EVO2513-0_5_0-lattech.kicad_sym — project symbol library (nickname Lattech Systems): the Lattech symbols used by the board, extracted from the schematics, plus the PCAL9714 added for the W16 changes. It is not the complete Lattech library, which was not supplied. Resistors and capacitors use KiCad's standard Device:R, Device:C and Device:C_Polarized symbols, with value, footprint and part number in the symbol fields, so a value change needs no new symbol
  • EVO2513-0_5_0-altium-import.kicad_sym — the 4 power symbols created by the Altium import. Both symbol libraries are registered in sym-lib-table.

Design changes (W16 review)

Part and value changes from the W16 schematic review. None changes a connection or the board copper.

RefWasNowWhy
Q1, Q3DMT4011LFG 40 VDMT6007LFGQ-7 60 VMargin against D1's clamp voltage
D11.5SMB27CA1.0SMBJ26CA (Diotec)Stand-off above the 24 V supply; 42.1 V clamp
L14.7 µH SRP1265A-4R7M10 µH SRP1265A-100MLTC1960's 10 µH minimum
C10100 nF 16 V100 nF 50 V CC0402KPX7R9BB104Sits on VPLUS at ~23 V
R541 kΩ768 Ω RC0402FR-07768RLSBC load-switch current limit (R22, R53, R71 stay 1 kΩ)
C16220 nF 50 V C0G 0805220 nF 50 V X7R CC0805KFX7R9BB224No 220 nF C0G 0805 exists
C39470 pF1 nFSW2 snubber, boost-mode ringing
C3, C11, C1235 V50 VDCFILTERED / DCBMS at 26.3 V
C44, C45, C48–C50, C5416 V50 V+12 V and the switched outputs
R1620K (description 619K)619KValue and description now agree
C2100 µF (part number 35SVPF82M)82 µF 35SVPF82MMatches the ordered part
C46, C47, C514.7 nF 50 V X7R 04021.8 nF 50 V X7R 0402 CC0402KRX7R9BB182TPS22811 DVDT caps (U6, U7, U9): shorter output ramp, as ordered for C47; the loads have little capacitance
R24–R2710 Ω0 ΩPack comms pass straight through; protection moves to the MCU board
D9, D10DT1240V3-04LP fittedDNPGo with R24–R27: wrong clamp level for 3.3 V, and the protected MCU is on another board
R140.01 Ω0.012 Ω Yageo PA2512FKE7W0R012EAdapter limit 8.33 A, below the 9.2 A supply, so charging throttles before the supply trips
R3661.9K fittedDNPVIN-FB goes to ground through R37, as required when PCM is unused
R59, R61, R76 / R60, R62, R771M / 130K390K / 51KTPS22811 PGTH dividers: 10.38 V threshold, string current 23.5 µA at threshold to meet TI's 20× PGTH leakage rule, so pin leakage can't push it near the rail
R67, R68, R812.2K4.7KPG LED (LED2–LED4) resistors from +3V3MCU: about half the current, ≈0.25 mA each instead of ≈0.55 mA, which saves ≈0.9 mA on battery with all three rails up. 4.7K is already on the BOM (R10)
R90–R92, R1011M1.07MOVLO trip 14.0 V, so a tripped switch recovers on the 12.03 V rail; R101 shares the BOM line
U6 EN/UVLOENDAQ from P0_0, R49 100K pull-downR108 619K / R49 75K UVLO divider, Q24 shutdown FET with R109 1.07M / R110 390K gate bias; net nENDAQ, active lowDAQ 11 V undervoltage lockout (W16 handoff §4.4)
R41, R452.2R 1% 1206, 1/4 W2.2R 1% 1210, 1/2 W (any standard thick film)Snubber resistors. R41 (SW1) dissipates 0.31 W at 24 V and 0.38 W at the 26.3 V OV trip, 75% of 1/2 W: fine up to about 90 °C local ambient. R45 (SW2) 0.167 W, 33%. Power is set by C·V²·f, not the load, so it is continuous at 1.157 MHz; power-save mode lowers it at light load. Same length as 1206; the pads are 0.45 mm wider each side
Q4, Q5, Q12–Q15DMP3018SFV, PowerDI3333-8 (Type UX), imported Altium landDMP3007SCG-13 (Diodes, V-DFN3333-8 Type B, 6.8 mΩ max at −10 V), Diodes_PowerDI3333-8, copied from KiCad's standard Package_SON library into the project library so it can carry the source-drain keepoutPowerPath/battery FET thermal margin (W16 handoff). KiCad has no Type B footprint; the PowerDI3333-8 one matches Diodes' Type B suggested land except 0.1 mm more toe on each pad row, and adds segmented paste on the drain. Its drain is one pad, 5, so the project symbol DMP3007SCG V-DFN3333-8 numbers D pins 5–8 and EP_D all 5. VGSS ±25 V as before. Diodes' datasheet (DS38990 rev 3-2) is still marked Advance Information
Q18CSD17304Q3unchanged (kept)The W16 handoff suggested a lower-RDS(on) 30 V part for the 1.83 W boost-mode loss. Kept: it works and 15 units are in field test. Its thermal margin depends on copper: 46 °C/W on 1 in² against 158 °C/W on a minimum pad, so give it the full copper area in layout
R160.005R 2512 (CRE2512-FZ-R005E-3)0.003R Bourns CRE2512-FZ-R003E-3The LTC1960 latching breaker (90–115 mV for 15 ms) moves from 18–23 A to 30–38 A. 12 V peak load is about 7.5 A SBC (90 W) + 2.5 A J3 + DAQ, over the handoff's ~11 A threshold, and QE29 packs at ~21 A would sit at 105 mV, inside the trip window. Dissipation at 21 A drops from 2.2 W to 1.3 W. R16 feeds only the breaker comparator (SCP/SCN)
R53, R711KunchangedDAQ and EXT current limits (6595/R = 6.6 A, up to 7.1 A) sit above J6/J5's single 6.5 A contact. Left at 1K: DAQ's final load isn't known (stand-in device today) and EXT is unused. A note on S07 says to raise them to 1.2K or more once the loads are known
D4Pins named as a series pairPins named for the fitted common-anode BAT54ADrawing and wiring were already right

Connection options on U5 (LM51772), as 0R 0402 links so either build can be fitted (lower right of S06): nRST stays on DCBMS in both BIAS builds.

PinFittedDNP (alternative)
MODE (7)R86 to GND: power-save mode (W16 review)R87 back to VCC2/ILIMCOMP: forced PWM, as built before
BIAS (40)R89 to +12V (U5's own output): the LM51772 datasheet's standard configuration (§7.3.5). VSMART runs the VCC2 regulator from the lower of VIN and BIAS once both exceed the switch-over threshold, so on the 24 V supply it drops from 12 V instead of 24 V; at start-up or with +12V shorted it falls back to VINR88 to DCBMS, as built on the field units

U5 is configured over I2C by default, not by its CFG resistors (parts right of the MODE/BIAS links on S06):

RefPartFunction in the I2C build (default)
R380R, CFG1 (ADDR/SLOPE, pin 9) to GNDSelects I2C at address 0x6A. 6.49K instead selects resistor configuration with slope compensation 1.0
R1040R, SDA/CFG3 (pin 5) to J3.34 MCU_ENDAQSDA to the MCU
R1050R, SCL/CFG4 (pin 6) to J3.36 MCU_ENEXTSCL to the MCU
R106, R10710K to +3V3MCUSDA and SCL pull-ups (pins rated to 5.8 V). 10K keeps edges slow for EMC and limits the bus to 100 kHz standard mode
R30, R295.1K and 1.87K to GND, DNPCFG3/CFG4 for the resistor build; fitted, they would load the bus

To return to the resistor build, remove R104–R107, change R38 to 6.49K and fit R29 and R30. J3.34 and J3.36 are also the direct-enable fallback through R97 and R98 (S08), so R97 and R98 stay unfitted while the I2C build is fitted. The MCU pins on J3.34/J3.36 must support I2C.

U5 starts from its register defaults, not the resistor settings, so firmware must write them before raising REGEN. They are latched for as long as DCBMS is up, since nRST is tied to DCBMS. Defaults that differ from the resistor build:

  • slope compensation is 0.875 (R38 selects 1.0)
  • VCC1, DRSS, hiccup mode and the current-limit options come from registers instead of R30 and R29
  • the internal DAC becomes the current-limit reference (ILIM_THRESHOLD); ILIMCOMP is tied to VCC2, so confirm the average current limit stays disabled
  • constant dead time (EN_CONST_TDEAD) defaults off; R30 (CFG3 setting 7) turns it on

Overvoltage lockout on the load switches U6, U7 and U9 (TPS22811, S07): a 1.07 MΩ 1% resistor (R90, R91, R92) from +12V to nEN/OVLO (pin 2), with the existing 100K 1% pull-downs R51, R52 and R70. Each switch turns off above 14.0 V (13.40–14.69 V over the ±2% pin threshold, 1% resistors and ±0.1 µA pin leakage) and turns back on below 12.75 V (12.23–13.41 V), so a tripped switch always recovers on U5's 12.03 V output. (1 MΩ gave 13.2 V, recovering at 11.50–12.60 V, which might not.) To revert, leave R90–R92 unfitted. The power-good dividers on PGTH are R59, R61 and R76 (390K) over R60, R62 and R77 (51K): PG rises at 10.38 V (9.62–11.17 V worst case) and falls at 9.43 V (8.71–10.22 V). They were 1M over 130K, but the ±1 µA PGTH leakage across 1M could put the threshold at 11.84 V, within 0.2 V of the rail. TI sizes the string for at least 20× the PGTH leakage (20 µA); 390K/51K carries 23.5 µA at the threshold and 27 µA at 12 V, and only while the switch is on, because the dividers hang off the switch outputs. 51K is already on the BOM. Undervoltage lockout on the DAQ switch U6 only: R108 619K from +12V over R49 75K on EN/UVLO (pin 1) turns U6 on at 11.10 V (10.63–11.91 V, including 1% resistors, ±0.1 µA pin and 0.5 µA FET leakage) and off at 10.09 V (9.69–10.89 V). TI asks for a pull-up of at least 350 kΩ on supplies above 5 V. 1M/120K would keep the 11.2 V point, but leakage across 1M puts the worst-case turn-on at 12.24 V, above the rail; 619K and 75K are already on the BOM and keep it under 12 V. The TPS22811's fixed hysteresis makes the turn-off point about 9% below turn-on, so 11 V has to be the turn-on point. Because the divider now holds EN/UVLO, the enable goes through Q24 (BSS138) from EN/UVLO to GND, and the expander net is nENDAQ, active low: high or floating (POR, expander in reset or unpowered) turns Q24 on and puts U6 in shutdown; low releases EN/UVLO to the divider. R109 1.07M / R110 390K bias the gate from +12V to 3.21 V (2.83 V at 10.6 V, 4.0 V worst case at the 14.7 V OVLO limit), so the channel stays off when the MCU board is unpowered, and the gate stays under 5 V. The divider draws 8.2 µA from +12V (it was 94 µA with 100K/27K), and both values are shared with other BOM lines. The gate's source impedance is 286K, so P0_1 can stay push-pull: driven high to 3.3 V it still holds Q24 on and sinks at most 2.4 µA, and the R97 fallback can drive it from a 3.3 V MCU pin. SBC and EXT have no UVLO. A note on S07 marks the DAQ circuit as deliberate.

If the UVLO causes trouble, R115 (0R, DNP) bypasses it. Fit R115 and remove Q24, R108 and R109: nENDAQ then drives EN/UVLO directly, as ENSBC and ENEXT drive U7 and U9, so P0_1 (or the R97 fallback) becomes active high and DAQ has no undervoltage lockout. R110 390K in parallel with R49 75K (62.9K) is the pull-down that holds U6 off while the expander is in reset or unpowered. Leaving R108 or R109 fitted with R115 would put a +12V divider on EN/UVLO, so remove both.

Rail enables and faults through a PCAL9714 SPI I/O expander (U11, new sheet S08). It shares CLOCK/MOSI/MISO with U1 (LTC1960) and has its own chip select, nCSIO, on J3.32, the pin that was ENSBC. Address 40h (ADDR to GND); INT has a pull-up but isn't routed off the board. Both supplies are +3V3MCU. RESET is held low by R100 (100K) and pulled to +3V3MCU by Q23 (BSS138, the same FET as Q20-Q22) whenever +12V is up: R99 100K / R101 1.07M put about 11 V on its gate. With the 12 V rail off the expander is in reset with every port an input, and RESET can never rise above +3V3MCU, so nothing back-powers the expander. The switch point depends on Q23's gate threshold (roughly 3.5-4 V on +12V with a BSS138) and has no hysteresis, so firmware should wait for +12V before configuring the expander.

Q20–Q23 are onsemi BSS138 (SOT-23) in place of the DMN65D8LFB-7 (DFN1006, 1.0 × 0.6 mm). Use the plain BSS138 or another part without a gate protection zener: the gates sit on 100K pull-ups (R63, R65, R78) and the R99/R101 divider, and ESD-protected parts such as the 2N7002K or BSS138BK leak up to about 10 µA, which would pull the PG high level down by about 1 V. BSS138: IGSS 100 nA, IDSS 0.5 µA, VGS(th) 0.8–1.5 V.

PortNetFunction
P0_0 (out)ENSBCU7 enable
P0_1 (out)nENDAQU6 enable through Q24, active low
P0_2 (out)ENEXTU9 enable
P0_4–P0_6 (in)PGDAQ, PGSBC, PGEXTU6, U7, U9 power good (also still drive the LEDs)
P0_7 (in)nFLTU5 nFLT/nINT, which was unconnected
P0_3, P1_0–P1_5—spare, not connected

REGEN (U5 enable, J3.12) stays separate: it is still driven straight from J3 and doesn't pass through the expander.

J3 pins 34 and 36 are now MCU_ENDAQ and MCU_ENEXT. Each reaches its enable only through a DNP 0R link (R97, R98), and J3.32 nCSIO has R95 (fitted) to the expander CS and R96 (DNP) to ENSBC. To go back to driving an enable straight from J3, fit its link and leave that expander port an input. The expander powers up with every port an input and pulls off, so the pull-downs (R50, R69) and Q24's gate bias keep the rails off until firmware sets P0_0–P0_2 as outputs. R97 now lands on nENDAQ, so an MCU driving DAQ directly must drive it low to enable. The MCU firmware must change for this: the three load-switch enables move from GPIO to SPI, and nCSIO must idle high (R93 pulls it up).

These parts aren't on the board yet: run Update PCB from Schematic, then place and route R86–R110, Q23, Q24, U11, C58 and C59, and re-place Q20–Q22 (now SOT-23). The ENDAQ, ENSBC and ENEXT tracks from J3 need cutting at the new links.

BOM consolidation

Parts with the same value in different packages or ratings now share one BOM line. Each change keeps or raises the voltage rating and tolerance. All resistors are 1%: the OVLO dividers moved from 1M/102K 0.1% to 1.07M/100K 1% (see the overvoltage lockout above), and R101 is 1.07M to share their BOM line.

RefsWasNow
C8, C91 µF 50 V X5R 04021 µF 50 V X5R 0603, as C23, C44, C45, C48–C50, C54
C7, C52, C53, C58, C59100 nF 16 V X7R 0402100 nF 50 V X7R 0402 CC0402KPX7R9BB104, as C10
C37, C38100 nF 16 V X7R 0603the same, 0402 (U5 bootstrap caps, ~5 V)
C17, C18, C20, C21, C34100 nF 50 V X7R 0402, no part numberCC0402KPX7R9BB104
C11–C14, C24–C2610 µF 25 V/50 V 120610 µF 50 V X7R 1210 Taiyo Yuden UMK325AB7106KMHP, as C27 (1210 is easier to source)
C2710 µF 50 V X5R 1210the same part, X7R
C16220 nF 50 V X7R 0805the same, 0603 Yageo AC0603KRX7R9BB224, as C22 (charger bootstrap cap)
C22220 nF 50 V 0603, material field X5RX7R, as its description already said
R43, R4410R 1% 060310R 1% 0402, as R4, R5, R24–R27 (U5 current-sense filter, no power)

Five U5 (LM51772) changes found during the review:

RefWasNowWhy
C30 → R10222 µF 6.3 V 0603 on VCC110K 1% 0402 to GND, as R7VCC1 is disabled (R30 5.1K on CFG3); the datasheet says tie a disabled VCC1 to GND through a resistor, not leave it floating
C3222 µF 6.3 V X5R 0603 on VCC222 µF 16 V X5R 0805 Murata GRM219R61C226ME15LVCC2 needs 6 µF minimum; the 0603 keeps only about 5–7 µF at 5 V
R291.9K1.87KCFG4 setting #3 accepts 1.814–1.926 kΩ (1.87K typical); 1.9K isn't a 1% value, and 1.91K can reach 1.929 kΩ
C61 (new)—100 nF 50 V X7R 0402 CC0402KPX7R9BB104 (as C34), BIAS (pin 40) to GND, between R88 and R89BIAS had no local decoupling; TI's WEBENCH design puts 100 nF (Cbias) on it. The +12V caps are about 4.6 mm away through R89
R46 (FB top)on the power-stage side of R48on +12V, teed into the ISNSN Kelvin trace from R48's load-side pad+12V is regulated after the 5 mΩ shunt, so it no longer sags by R48's drop (about 55 mV at 11 A). Matches the datasheet's Figure 9-1 and §9.9.1.3 (route the top feedback resistor to the output sense point). VOUT (pin 18) stays on the power stage

Run Update PCB from Schematic to swap the footprints. Parts that grow overlap their neighbours' courtyards and need moving: the 0603s for C8 and C9 by up to 0.9 mm (C8 against R8, C9 against R15 and C10), the 1210s by about 0.15 mm (C11/C12/C27, C24/C26, C25 against C23), and C32 by 0.3 mm against C38 (before C38 shrinks to 0402) and 0.1 mm against TH2.

Manufacturer part numbers

MANUFACTURER and MANUFACTURER_PN are filled on every fitted part, in the schematic and on the board. Parts unchanged since 0.5.0 carry the exact part numbers bought for the 0.5.0 backup build (DigiKey list for 20 boards, plus a Mouser order for LM51772RHAR, DMT6007LFGQ-7 and DMT4011LFG-7). Parts that changed reuse a bought part where value, package and rating match (for example the 390K/51K PGTH dividers take the R9 51K part). Parts with no earlier order keep the schematic's part number, or take a Yageo RC/CC-series part: RC0402JR-070RL (0R), RC0402FR-07390KL, RC0402FR-071M07L, RC0402FR-071K87L, RC1210FR-072R2L, CC0805KPX7R9BB102, CC0603KRX7R9BB104. Resistors are standardised on Yageo (R31 RC0402FR-1340K2L, R111–R114 RC0603FR-073RL), except the current-sense shunts R16, R19, R42 and R48. D6–D8 are B340A-13-F. M1–M6 have no manufacturer fields; their value is the Würth part number.

Five lines use parts held in stock from the 0.5.0 orders, with the earlier schematic part kept in the NOTE field as Alternate: <manufacturer> <part number>:

RefFitted partAlternate (NOTE)
C6Yageo CC0402KRX7R9BB182 1.8 nF 50 V X7R, as C46, C47, C51KEMET C0402C182K4RACTU
C8, C9, C23, C44, C45, C48–C50, C54Samsung CL10A105KB8NNNC 1 µF 50 V X5R 0603Murata GRT188R61H105KE13D (AEC-Q200)
C15KEMET C0805C475K8PACTU 4.7 µF 10 V X5R 0805Murata GRM219R61A475KE34J
D2MCC MBR0540-TPPanjit SS0540_R1_00001
L2Würth 744393580068 0.68 µH, on the XAL8080 footprintCoilcraft XAL8080-681MEB

Fixes after import

Each fix is a separate commit on top of the initial import.

Problem in the raw importFix
Every symbol's Value field was ${ALTIUM_VALUE}, resolved through a per-symbol fieldCopied the real value into Value (209 symbols); the 26 test points, which had no value, are POGO-1
12 Footprint fields differed from the placed footprint only in letter case, so library lookup failedFields now name the exact footprint used on the PCB (J2, J5, J6, M2–M6, FL1, D9, D10, L2)
An imported FOOTPRINT field holding the bare package name (0402, SMA, …) overrode the real Footprint field, since KiCad matches field names case-insensitivelyRenamed to ALTIUM_FOOTPRINT on all 237 symbols
Altium net labels became KiCad local labels, which don't connect across sheets, splitting 35 netsConverted the 78 labels for those nets to global labels
44 embedded library symbols drew Altium special strings =Value and =FootPrint as literal text=Value replaced with ${VALUE}; =FootPrint replaced by showing each part's own ALTIUM_FOOTPRINT field in the same place, so parts show their part number and package as in Altium
All 99 power symbols were unannotated (#PWR?)Annotated #PWR1–#PWR99
The "Lattech Systems" symbol library wasn't available, so symbols existed only as copies embedded in the schematics, some in several slightly different versionsExported the symbols to project libraries under their original library names, and made every schematic use one definition per symbol
Chip resistor and capacitor footprints had poor pads (0402s used 0.635 mm circular pads) and caused tombstoningReplaced all 139 with KiCad standard IPC-7351 nominal footprints (Resistor_SMD, Capacitor_SMD) in place: same position, rotation and nets, zones refilled
Diodes and LEDs used imported Altium lands where KiCad has a standard IPC-7351 footprint; the LED land carried A/C silk text below the minimum thickness (8 DRC warnings)Swapped to KiCad standard footprints in place (same position, side and nets; pad centres within 0.33 mm): D1 Diode_SMD:D_SMB, D6–D8 Diode_SMD:D_SMA, D4 Package_TO_SOT_SMD:SOT-23 (as Q20–Q24), D9/D10 Package_DFN_QFN:Diodes_UDFN-10_1x2.5mm_P0.5mm (identical pads), LED1–LED4 LED_SMD:LED_0603_1608Metric, turned 180° because its pad 1 (cathode) is on the other side. The SMA/SMB pads are 0.6–0.7 mm longer towards the body. The power FETs keep their imported lands: they match the manufacturers' suggested layouts, KiCad's equivalents number the whole drain as one pad, and Q18's land is proven on the field units. The five unused imported footprints are removed from the project library
PCB footprints were linked to the imported symbols by mismatched internal IDs, and nets used Altium namesRan Update PCB from Schematic: no errors, placement and copper unchanged, all 147 nets match the schematic
KiCad design rules were defaults (0.2 mm clearance and track, 0.3 mm min hole), not the Altium rulesSet to the rules in the Altium .PcbDoc: 0.15 mm clearance, track and annular ring, 0.15 mm min hole, 0.3 mm hole-to-hole, and EVO2513.kicad_dru for the 0.3 mm pad-to-pad rule on test points TP1–TP26
The import turned 347 Altium copper regions into board graphic polygons (gr_poly) on B.Cu and In1–In6: a 1.2 × 1.8 mm octagon over each six-via block, on every layer. As drawings they bypass zone clearance and fill rules, and on the GND layers most were net islands in the GND pour, including the charger switch node (Net-(D2-C))Removed all of them. None carried current: each only joined its own vias, which every same-net pour already connects solid, and DRC finds 0 unconnected without them. GND gains about 26 mm² on In1, 21 mm² on In3 and In5, 18 mm² on In6 and 27 mm² on B.Cu
FL1's ground land had no pad number, so its 38 GND vias showed as shortsNumbered pad 4 (GND) on the board and in the project footprint library
The two mounting holes and the logo existed only on the board, with no schematic symbolsH1 and H2 (Mechanical:MountingHole_Pad, pin 1 to GND, project footprint MountingHole_3.2mm_Pad_7.4mm) and LOGO01 (EVOSONIC_LOGO, a pinless symbol in the Lattech library) are on the root sheet, excluded from BOM and position files. Update PCB from Schematic no longer deletes them
14 zero-length track segmentsRemoved
FL1's courtyard had a centre cross drawn on F.CrtYd, so KiCad saw an open (malformed) courtyardMoved the cross to F.Fab on the board and in the project footprint library
Two vias sat in 0402 pads (R13 pad 2, R54 pad 2), connected on F.Cu only, and could wick solderRemoved
9 tracks ran within 0.15 mm of the new R/C pad corners, B.Cu tracks passed 0.10 mm from J2 pins 9/10, and the ENEXT track 0.21 mm from J3's peg holeRerouted; 15 small R/C parts and 3 GND vias moved 0.1 mm
Net class patterns named Altium's auto-generated nets, so 13 power nets were in the Default classPatterns point at the current net names
Every sheet sat 43 mil off the 50 mil connection grid in YShifted each sheet's contents 7 mil onto the grid, and moved the few remaining off-grid wire corners on S06 onto it
9 wires ran past their labels, leaving dangling endsTrimmed back to the label
GND, +12V, +3V3MCU and +5V had no power source for ERCAdded PWR_FLAG symbols
Title blocks used the Altium formula ${COPY(DOCUMENTNAME,…)} for the sheet titleReplaced with each sheet's title
Every resistor and capacitor had its own per-value Lattech symbol (76 of them), and the schematic showed the ALTIUM_VALUE field, not Value, so R1, C39 and R54 still displayed their old valuesSwapped all 160 for KiCad's Device:R, Device:C and Device:C_Polarized (C2, C28, C40–C42) in place, connections unchanged; Value is now the displayed field, and the 76 symbols are gone from the project library. ALTIUM_VALUE brought in line with Value on R1, C39, R54, D1, Q1, Q3 and L1
The import made seven KiCad 10 top-level sheets, so kicad-cli only loaded S01, and every title block read "sheet 7 of 7"Added a root sheet with the seven as sub-sheets (S01's content moved to S01 External Connectors.kicad_sch); sheet numbers now come from the page number

Symbols still carry their imported Altium fields (ALTIUM_VALUE, ALTIUM_FOOTPRINT, MANUFACTURER, MANUFACTURER_PN, …) for reference.

Known remaining issues

  • The KiCad default title block is drawn over the imported Altium one.
  • DRC reports 15 warnings and no errors: silkscreen overlaps, where the connector tab labels sit on the J1, J2 and J4–J6 outlines. 19 hits are excluded: 16 board-edge clearance hits from the layer-order markers, which cross the edge on purpose, and M6's three starved thermal reliefs (below).
  • The mounting spacers M1–M6 connect to GND through pad thermal reliefs set in the footprint (MECH SPACER WURTH 78614150960 THROUGH M3, also on the board): four 2 mm spokes at 0/90/180/270° across a 0.4 mm gap. These replace the four keepout arcs inherited from Altium, which gave about 1.43 mm spokes and left dead copper stubs wherever a sector faced the board edge or another net's pour. Spokes are only drawn where they reach the pour, so M1–M5 have 2–3 per layer, as many live connections as before, with about 40 % more connected copper. M6 sits between the DCCHARGER and DCPATH pours, so it connects through In1 and B.Cu (4 spokes each) and one spoke on In3, In5 and In6, where DRC's two-spoke minimum is excluded. A rule in EVO2513.kicad_dru keeps other nets' pours 0.45 mm from M6.
  • Every power FET footprint (Q1, Q3–Q19) has a top-copper keepout (no pour, tracks or vias) across the gap between its source/gate row and its drain pad, so the gap is bare laminate as in the manufacturers' land patterns, not just solder mask over a pour. EVO2513.kicad_dru also keeps other nets' pours 0.3 mm from those FETs' pads. Both protect the source-drain gap during rework.
  • DNP parts get no solder paste: a rule in EVO2513.kicad_dru gives every footprint marked DNP a −50 mm paste margin, so its stencil apertures drop out of F.Paste. Clearing a part's DNP flag restores its paste. KiCad has no plot option for this.
  • R111–R114 (3R 0603) are series gate resistors on Q16–Q19, as R7–R10 (3.0 Ω) on TI's LM51772EVM-HP, to slow the switching edges for EMI. Each sits next to its FET's gate pad, and the gate drive comes up from In6 through a via in the resistor's driver-side pad. R113 and R114 sit side by side between Q19 and Q18, and R112 sits north of Q17's gate between R84 and C28. Fit 0R to restore direct drive. Worst-case dissipation is about 45 mW each at 1.157 MHz and 5 V drive.
  • The switch-node snubbers tie in at their low-side FETs, in the same order as TI's LM51772EVM-HP: switch node, then capacitor, then resistor, then GND. That way only the small 0805 capacitor pad sits on the switch node. C39's SW2 pad sits on Q19's drain edge, with C39 and R45 running north past L2 to R45's GND pad and two vias to In1. C35's SW1 pad sits on Q17's drain leads, with C35 and R41 in the strip between Q19 and Q17 and two vias to In1 at R41's GND pad. The return runs on In1 directly under each chain. The top-copper SW1 and SW2 pour lobes that used to reach the old positions by L2 were removed. Each snubber resistor dissipates C × V² × f while its node switches. R41 takes 0.31 W at 24 V in buck mode (0.37 W at 26 V) and R45 0.17 W in boost mode, at 1.157 MHz, in 0.5 W 1210 parts. TI's LM51772EVM-HP uses 680 pF with 3 Ω 0.1 W 0603 resistors at 600 kHz, which dissipate 0.24 W at 24 V and 0.16 W in boost: similar power, with a fifth of the rating.
  • C60 (100 nF 50 V X7R 0603) is the high-frequency output capacitor for the boost hot loop, as C7 on TI's LM51772EVM-HP. It sits directly south of Q18's drain tab, with a via in its output pad to the inner output planes and two vias in its GND pad to In1, which runs solid GND 0.094 mm under the top layer, so the return current follows the top-layer path back to Q19's source.
  • R115, the DNP UVLO bypass for U6, is on the top side east of Q24, below R108, with both connections on top copper: pad 2 to Q24's gate (nENDAQ) and pad 1 to the EN/UVLO track from R108.
  • The design relies on via-in-pad: over 700 vias sit in pads (FET tabs, QFN exposed pads, FL1, the 2512 shunts, and 0402/0603 capacitors). Order the board with vias filled and capped; open vias would wick solder from the small pads.

Generated outputs (netlists, backups, per-user .kicad_prl settings) are not tracked; see .gitignore.

Parts

271
QtyValueFootprintReferences
26POGO-1EVO2513-0_5_0-import-fps:TEST PIN 1-25mm SMD Pad (POGO-1)TP1, TP2, TP10, TP11, TP12, TP13, TP14, TP15, TP16, TP17, TP18, TP19, TP20, TP21, TP22, TP23 +10
160RResistor_SMD:R_0402_1005MetricR24, R25, R26, R27, R38, R86, R87, R88, R89, R95, R96, R97, R98, R104, R105, R115
14100KResistor_SMD:R_0402_1005MetricR3, R12, R18, R40, R50, R51, R52, R63, R65, R69, R70, R78, R99, R100
14100nFCapacitor_SMD:C_0402_1005MetricC7, C10, C17, C18, C20, C21, C34, C37, C38, C52, C53, C58, C59, C61
1210KResistor_SMD:R_0402_1005MetricR7, R28, R55, R56, R72, R73, R75, R93, R94, R102, R106, R107
91uFCapacitor_SMD:C_0603_1608MetricC8, C9, C23, C44, C45, C48, C49, C50, C54
810uFCapacitor_SMD:C_1210_3225MetricC11, C12, C13, C14, C24, C25, C26, C27
6100RResistor_SMD:R_0402_1005MetricR15, R21, R64, R66, R79, R80
678614150960EVO2513-0_5_0-import-fps:MECH SPACER WURTH 78614150960 THROUGH M3M1, M2, M3, M4, M5, M6
6DMP3007SCG-13EVO2513-0_5_0-import-fps:Diodes_PowerDI3333-8Q4, Q5, Q12, Q13, Q14, Q15
6DMT4011LFGEVO2513-0_5_0-import-fps:Power DI3333-8 B3.3 x 3.3 P0.65 Tab 8-PinQ6, Q7, Q8, Q9, Q10, Q11
51.07MResistor_SMD:R_0402_1005MetricR90, R91, R92, R101, R109
551KResistor_SMD:R_0402_1005MetricR9, R11, R60, R62, R77
5BSS138Package_TO_SOT_SMD:SOT-23Q20, Q21, Q22, Q23, Q24
5NEQResistor_SMD:R_2512_6332MetricR23, R82, R83, R84, R85
41.8nFCapacitor_SMD:C_0402_1005MetricC6, C46, C47, C51
410RResistor_SMD:R_0402_1005MetricR4, R5, R43, R44
4390KResistor_SMD:R_0402_1005MetricR59, R61, R76, R110
43RResistor_SMD:R_0603_1608MetricR111, R112, R113, R114
44.7KResistor_SMD:R_0402_1005MetricR10, R67, R68, R81
4QTLP600C-4LED_SMD:LED_0603_1608MetricLED1, LED2, LED3, LED4
3180uFEVO2513-0_5_0-import-fps:CAP Panasonic CASE-E12C40, C41, C42
31KResistor_SMD:R_0402_1005MetricR22, R53, R71
321.5KResistor_SMD:R_0402_1005MetricR57, R58, R74
35.1KResistor_SMD:R_0402_1005MetricR6, R13, R30
3619KResistor_SMD:R_0402_1005MetricR1, R17, R108
3B340ADiode_SMD:D_SMAD6, D7, D8
3TPS22811EVO2513-0_5_0-import-fps:VQFN-HR B2.0x2.0x1.0 10-Pin TI LM73100RPWU6, U7, U9
2100pFCapacitor_SMD:C_0402_1005MetricC19, C57
21053091102EVO2513-0_5_0-import-fps:CONNECTOR MOLEX 1053091102 2POS 2.5MM THPJ5, J6
210kResistor_SMD:R_0603_1608MetricTH1, TH2
22.2RResistor_SMD:R_1210_3225MetricR41, R45
2220nFCapacitor_SMD:C_0603_1608MetricC16, C22
25.62KResistor_SMD:R_0402_1005MetricR37, R47
275KResistor_SMD:R_0402_1005MetricR33, R49
2DMT6007LFGQ-7EVO2513-0_5_0-import-fps:Power DI3333-8 B3.3 x 3.3 P0.65 Tab 8-PinQ1, Q3
2DT1240V3-04LPPackage_DFN_QFN:Diodes_UDFN-10_1x2.5mm_P0.5mmD9, D10
2FiducialEVO2513-0_5_0-import-fps:Fiducial-50Fiducial1, Fiducial2
2IAUCN04S7L019EVO2513-0_5_0-import-fps:Infineon_PG-TDSON-8-33_5.48x5.15mm_P1.27mmQ16, Q19
2M3EVO2513-0_5_0-import-fps:MountingHole_3.2mm_Pad_7.4mmH1, H2
2TLV9002IDSGEVO2513-0_5_0-import-fps:WSON B2x2 P0-5 8-Pin EPU8, U10
10.0015RResistor_SMD:R_2512_6332MetricR42
10.003RResistor_SMD:R_2512_6332MetricR16
10.005RResistor_SMD:R_2512_6332MetricR48
10.012RResistor_SMD:R_2512_6332MetricR14
10.015RResistor_SMD:R_2512_6332MetricR19
10.68uHEVO2513-0_5_0-import-fps:IND COILCRAFT XAL8080L2
11.0SMBJ26CADiode_SMD:D_SMBD1
11.87KResistor_SMD:R_0402_1005MetricR29
1100nFCapacitor_SMD:C_0603_1608MetricC60
110144517-043802LFEVO2513-0_5_0-import-fps:Connector Amphenol BergStak 10144517-043802LF 40-Pin RecepticalJ3
11053101114EVO2513-0_5_0-import-fps:CONNECTOR MOLEX 1053101114 2.5MM THPJ2
11053101204EVO2513-0_5_0-import-fps:Connector Molex 105310xx04 4POS 2.5mm THPJ1
11053102204EVO2513-0_5_0-import-fps:Connector Molex 105310xx04 4POS 2.5mm THPJ4
110nFCapacitor_SMD:C_0402_1005MetricC5
110uFCapacitor_SMD:C_0603_1608MetricC56
110uHEVO2513-0_5_0-import-fps:IND Bourns SRRP1265AL1
1110pFCapacitor_SMD:C_0402_1005MetricC36
1120uFEVO2513-0_5_0-import-fps:CAP Panasonic CASE-F12C28
112KResistor_SMD:R_0402_1005MetricR2
113KResistor_SMD:R_0402_1005MetricR34
115nFCapacitor_SMD:C_0402_1005MetricC33
1180pFCapacitor_SMD:C_0402_1005MetricC31
11nFCapacitor_SMD:C_0805_2012MetricC39
11nFCapacitor_SMD:C_0402_1005MetricC4
12.2uFCapacitor_SMD:C_1206_3216MetricC3
12.7KResistor_SMD:R_0402_1005MetricR35
122uFCapacitor_SMD:C_0805_2012MetricC32
122uFCapacitor_SMD:C_1210_3225MetricC43
127KResistor_SMD:R_0402_1005MetricR39
13.6KResistor_SMD:R_0402_1005MetricR20
14.22KResistor_SMD:R_0402_1005MetricR32
14.7nFCapacitor_SMD:C_0402_1005MetricC1
14.7uFCapacitor_SMD:C_0805_2012MetricC15
140.2KResistor_SMD:R_0402_1005MetricR31
1470pFCapacitor_SMD:C_0805_2012MetricC35
161.9KResistor_SMD:R_0402_1005MetricR36
162KResistor_SMD:R_0402_1005MetricR46
1680KResistor_SMD:R_0402_1005MetricR8
168nFCapacitor_SMD:C_0402_1005MetricC29

The 253 most common of 271 parts.

Similar boards

  • 4 layers100 × 100 mmRpi pico printer board, the printed circuit board in 3D

    Rpi pico printer board

    jackw01/pi-pico-printer-board

    Tinkerer-friendly Klipper compatible 3D printer control board using Raspberry Pi Pico

    224 parts42CERN-OHL-W-2.0
  • 4 layers92 × 95 mmESP32-CAN, the printed circuit board in 3D

    ESP32-CAN

    Eric-2012/ESP32-CAN

    251 parts5
  • 10 layers224.5 × 160 mmHaasoscope pro adc fpga board, the printed circuit board in 3D

    Haasoscope pro adc fpga board

    drandyhaas/HaasoscopePro

    Affordable 2 GHz 3.2 GS/s 12 bit open-source open-hardware expandable USB real-time oscilloscope

    586 parts485MIT
  • 2 layers155 × 80 mmESP32Controller, the printed circuit board in 3D

    ESP32Controller

    simon-jouet/ESP32Controller

    ESP32-based 3D printer controller

    171 parts134
  • 4 layers50 × 60 mmPiCCANTE OBD Dongle, the printed circuit board in 3D

    PiCCANTE OBD Dongle

    Alia5/PiCCANTE

    PiCCANTE is a powerful tool for exploring and reversing CAN busses of vehicles, based on Raspberry Pi Pico (any model)

    35 parts104GPL-3.0
  • 4 layers110 × 110 mmSmoothiev2-prime, the printed circuit board in 3D

    Smoothiev2-prime

    Smoothieware/Smoothieboard2

    Hardware files for the Smoothieboard v2, and extension boards

    453 parts71
  • 2 layers105.2 × 71.1 mmOnyx PCB, the printed circuit board in 3D

    Onyx PCB

    CuriousMotor/Onyx-Stepper-Motherboard

    The successor of the iconic Arduino-CNC-shield

    96 parts56MIT
  • 2 layers75.8 × 92.5 mmESP32 STEPPER CONTROL PCB, the printed circuit board in 3D

    ESP32 STEPPER CONTROL PCB

    JohnDecebal/UNDR

    UNDR AUTO is a fully automatic WDT (Weiss Distribution Technique) tool designed for espresso enthusiasts. This open-source DIY project combines 3D printed parts with electronic and mechanical components to create a…

    48 parts46

Questions

How big is the EVO2513 PCB?

It measures 110 × 69 mm and has 8 copper layers, 1.59 mm thick.

What parts does the EVO2513 use?

271 parts, built around the TLV9002IDSGR, DMT4011LFG, BSS138 and QTLP600C4TR. The full list of its parts is on this page, with links to each part's symbol and footprint where PCBKit's library has them.

Where can I download the EVO2513 KiCad files?

From the evosonic/evoone-bms-pcb repository on GitHub, at the commit this page was made from: the board is EVO2513.kicad_pcb and its schematic EVO2513.kicad_sch. PCBKit opens the board in the browser, with nothing to install.

Can I use the EVO2513 design in my own project?

Its repository states no licence, so its author keeps all rights: ask evosonic before reusing the design.