L96-M33 PCB example

IoT Modules GNSS Module
1

I’m designing the pcb for a L96-M33 with internal antenna, it would be very helpful if you could provide me with a kicad example with a tested ground plane

2

Hi @Hal you may refer to below link for the documentation related to L96 module design:

  1. https://www.quectel.com/download/quectel_l96_hardware_design_v1-4/
  2. https://www.quectel.com/download/quectel_l96_reference_design_v1-1/
  3. https://www.quectel.com/download/quectel_l96_footprintpart_20171206-2/

Best regards,

3

Hi, I didn’t explain myself clearly. The documentation you sent me is the same as the one on your website. The only reference to what I need is chapter “4.3. PCB Layout Suggestion,” which contains an image of a cross-section of one side of your demo board. I need an example of a board that includes the chip’s internal antenna with a ground plane of 80mm x 40mm. Given the possibility of ground loops and other issues, I asked if it had also been tested in a real-world scenario. Best regards.

4

Hi @Hal

Thanks for clarifying — the cross-section in Ch. 4.3 is the L96 EVB layout, just rendered as a
generic diagram. Here is the actual reference board with the 80mm × 40mm ground plane that
has been characterized for real-world performance.

— Figure 19: PCB Layout (L96 HW Design V1.4 Ch. 4.3) —

img_v3_02148_d74c3bdd-a9df-4ba8-ba05-5dd4ef8951ag
img_v3_02148_d74c3bdd-a9df-4ba8-ba05-5dd4ef8951ag1044×594 110 KB

— L96 EVB Top View (the production reference board) —

img_v3_02148_9dde236d-c077-4b84-b40b-624ebcfde8fg
img_v3_02148_9dde236d-c077-4b84-b40b-624ebcfde8fg1172×710 94 KB

— L96 EVB Bottom View (shows the 4-layer ground plane implementation) —

img_v3_02148_84ff7843-aa8b-4500-b584-64818e1911dg
img_v3_02148_84ff7843-aa8b-4500-b584-64818e1911dg1040×754 64.7 KB

The 80mm × 40mm ground plane is the documented OPTIMUM size (not the minimum). The L96 EVB
is the production-tested reference design that uses this exact configuration. All performance
figures in the datasheet (e.g. -165 dBm tracking sensitivity) are characterized on this board.

For the ground-loop concern, please follow these layout rules (L96 HW Design V1.4 Ch. 4.3):

• 10mm minimum clearance between the module edge and the nearest ground plane edge
• Keepout area (4.8mm × 7.3mm) above the patch antenna — no copper, no components
• For 2-layer PCB: continuous ground plane on the opposite side from the module, no
traces cutting through under the module
• For 4-layer PCB (recommended): make Layer 2 a complete ground plane. This isolates the
power and signal layers from the RF section and prevents ground loops between noisy
circuits (battery, MCU, etc.) and the antenna ground reference
• Match RF trace impedance to 50Ω (only if routing from internal antenna to external RF_OUT)
• Place the module at the center of the top edge of the motherboard

For the full reference design, please use:
• Quectel_L96_Reference_Design_V1.1 (schematic of the production EVB)
• Quectel_L96_EVB_User_Guide_V1.2 (tested design with TTFF, antenna interface, PowerGPS procedure)
• Quectel_L96_2D_Dimensions_V1.0 / 3D_Dimensions_V1.0 (PCB layout files)
• Quectel_L96_Footprint&Part_20171206 (Altium footprint + 3D model)

All available from the Quectel product page: https://www.quectel.com/product/gnss-l96
(under “Hardware Development Resources”)

Best regards,

5

It’s clear now, thanks.