Electronics JTAG Module Board Layout - thepinkmile/Enigma-NG GitHub Wiki

JTAG Module Layout Visualisations

Status: In Review Project: Enigma-NG Author: Izzyonstage & GitHub Copilot Version: v.0.1.0 Associated Hardware Revision: Rev A Last Updated: 2026-05-20

This board implements our version of an Intel (Altera) USB Blaster II device for programming CPLDs.

1. Component Areas

TOP VIEW (L1) - 4-Layer (DEC-017) / 2oz Copper
 _______________________________________________________________________________________
|                                                                                       |
|   [ MH1 ]                                                   [ MH2 ]                   |
|   (Top-Left, M2.5 NPTH, 7mm from edge)                     (Top-Right, M2.5 NPTH)     |
|                                                                                       |
|   [ FT232H IC ] <--- High-Speed USB to MPSSE Bridge                                   |
|   (Main IC for JTAG Blaster, 12MHz Crystal Attached)                                  |
|                                                                                       |
|   [ DATA PLATE ] <--- Inverted White Silkscreen on L4 (B.Silkscreen / exterior face)  |
|   (Enigma Silhouette + JLC Serial)                                                    |
|                                                                                       |
|    [ MH3 ]                     [ J1 DF40 ]                    [ MH4 ]                 |
|   (Bot-Left, inset 12mm)       (Bottom-Centre, 20-pin BtB)    (Bot-Right, inset 12mm) |
|_______________________________________________________________________________________|

2. Simplified Layout

 ________________________________________________ 
|  [MH1]                               [MH2]     |
|                                                |
|          [ FT232H + supporting components ]    |
|                                                |
|  [MH3]         [ J1 DF40 BtB ]         [MH4]   |
|_________________(Bottom-Centre)________________|

Connector Definition Owner: This board. All other boards connecting to the JTAG Module cross-reference here.

3. J1 DF40C-20 BtB Connector Pinout (20-Pin, Bottom-Centre)

Part: Hirose DF40C-20DP-0.4V(51)
Location: Bottom-centre of board; R1 row on the outer (bottom) board edge.
Mating part (CTL J12): Hirose DF40HC(3.5)-20DS-0.4V(51) — 3.5mm stack-height receptacle on CTL board.

       C1     C2     C3     C4     C5     C6     C7     C8     C9    C10
  R1:  TCK    GND    GND   5V_U   GND    GND   3V3    GND    GND    TDI
  R2:  GND    TMS    GND    GND   USB+   USB-   GND    GND    TDO    GND

R1 = outer (bottom) edge; R2 = inner row.

Pin Signal Dir Description
C1R1 TCK JM → CTL JTAG Clock (buffered via U2; 33Ω via R2)
C2R1 GND — Ground
C3R1 GND — Ground
C4R1 5V_USB CTL → JM 5V USB power from CTL TPS2065C rail
C5R1 GND — Ground
C6R1 GND — Ground
C7R1 3V3_ENIG CTL → JM 3.3V logic rail / JTAG signal reference
C8R1 GND — Ground
C9R1 GND — Ground
C10R1 TDI JM → CTL JTAG Data In (33Ω via R4; R1 at FT232H)
C1R2 GND — Ground
C2R2 TMS JM → CTL JTAG Mode Select (buffered via U2; 33Ω via R3)
C3R2 GND — Ground
C4R2 GND — Ground
C5R2 USB+ Bidir USB 2.0 D+ to CM5 (USB FS differential pair)
C6R2 USB− Bidir USB 2.0 D− to CM5 (USB FS differential pair)
C7R2 GND — Ground
C8R2 GND — Ground
C9R2 TTD_RETURN CTL → JM JTAG Transmission Data return from chain end
C10R2 GND — Ground

4. PCB Stackup — see GRS §2.3.2

Stackup: see GRS §2.3.2

Layer Role Notes
L1 GND plane + SMT component pads (component side) Faces toward Controller Board when JM is mounted as a hat
L2 All signal traces (inner layer) Shielded between L1 GND reference and L3 power
L3 Power distribution pours (5V_USB + 3V3_ENIG) Inner power layer
L4 GND pour shield Faces away from Controller (exterior/top when mounted)

5. Grounding Notes

GND_CHASSIS is not implemented on the JM - see DEC-057. Mounting holes connect to GND (circuit return).

6. Routing - Trace Width Specifications

Board specs: 4-layer / 2oz finished copper (inverted) — stackup per GRS §2.3.2. L1 = GND plane (component side); L2 = all signal traces (inner layer); L3 = power pours; L4 = GND pour.

IPC-2221A basis (2oz copper, 10°C rise, 25°C ambient): External: ~0.15 mm/A. Internal: multiply by 2.5x for same thermal rise. See design/Standards/Global_Routing_Spec.md §1.1 for the full current-category table.

6.1 Trace Width Table

Net Peak Current IPC Calc (2oz) Design Min Specified Width Layer Notes
5V_USB (J1 C4R1 → FT232H VCC) ≤ 120 mA peak 0.02 mm per GRS §1.1 per GRS §1.1 L1 + L3 pour FT232H datasheet Table 5.2 (p.41): Ireg ≈ 54 mA + Iccphy ≈ 60 mA = 114 mA absolute max, rounded up to 120 mA for margin. Note: a legacy figure of 400 mA was ≈4× the actual device maximum and has been corrected. Power-rail minimum applies.
3V3_ENIG (J1 C7R1 → FT232H VCCIO) 15 mA 0.002 mm per GRS §1.1 per GRS §1.1 L1 + L3 pour VCCIO domain; 3V3_ENIG canonical width per GRS §1.1
JTAG signals: TCK, TMS, TDI, TDO (CI) signal - per GRS §2.3.2 per GRS §2.3.2 / JLCPCB_Manufacturing.md §1.1 L2 (inner) JM inverted stackup (DEC-017): L2 buried microstrip immediately below L1 GND plane. 50 Ω controlled impedance per GRS §2.3.2 and JLCPCB_Manufacturing.md §1.1. Per DEC-016.
USB D+ / D- differential pair signal — see GRS §2.3 see design/Production/JLCPCB_Manufacturing.md §1 L2 (inner) 90 Ω differential USB 2.0; must be length-matched to within 0.1 mm; routed as a tightly-coupled pair
GND pours (outer layers) - - pour copper pour L1 + L4 Both outer layers = solid GND; provides dual-sided shielding for L2 signals
Power pours (inner power layer) ≤ 120 mA - pour copper pour L3 Separate pour zones for 5V_USB and 3V3_ENIG

6.2 Notes

  • All JTAG traces on L2 are sandwiched between the L1 GND reference (top) and L3 power pour (bottom), providing inherent shielding and a well-defined impedance environment.
  • JTAG CI traces: 50 Ω controlled impedance on L2 (buried microstrip, immediately below L1 GND plane per DEC-017 inverted stackup). Trace width per GRS §2.3.2 and design/Production/JLCPCB_Manufacturing.md §1.1.
  • USB D+/D- trace width and differential impedance shall comply with design/Production/JLCPCB_Manufacturing.md §1 and design/Standards/Global_Routing_Spec.md §2.3 for the board's assigned stackup.

7. Mounting Holes

JM mounting holes MH1–MH4 are M2.5 NPTH holes with a GND annular ring. Net: GND (not GND_CHASSIS — daughterboard exception per DEC-057). No purchasable BOM component on the JM; mounting standoffs are owned and sourced by the Controller Board BOM (MH9–MH12, 9774035151R, M2.5×3.5mm SMT standoffs). See design/Standards/Global_Routing_Spec.md §4 for module mounting hole rules. See DEC-057 (standoff ownership) and DEC-058 (JM BtB upgrade) for full rationale.

MH1–MH4 Pattern

Hole Location From Left From Right From Top From Bottom
MH1 Top-left corner 7 mm — 7 mm —
MH2 Top-right corner — 7 mm 7 mm —
MH3 Bottom-left inset 12 mm — — 7 mm
MH4 Bottom-right inset — 12 mm — 7 mm

Notes:

  • MH1 and MH2 are right in the top corners for maximum mechanical stability above the DF40 connector.
  • MH3 and MH4 are inset from the bottom corners (12 mm from each side) to leave space for J1 (DF40) centred between them at the bottom edge.
  • Final board dimensions are deferred to PCB layout time (same approach as AM board).
  • Positional asymmetry (MH1/MH2 at 7 mm, MH3/MH4 at 12 mm from sides) enforces correct orientation, combined with silkscreen pin-1 markers on J1.