0.4mm Fine Pitch BGA PCB Design Guidelines

Nowadays, more and more precise electronic components are widely used in some advanced electronics devices, such as fine pitch FPGA component from Xilinx. But accordingly this take extra challenges to PCB designer and PCB manufacturing’s capability when the design has many limits in spacing of tracks, plated holes, electronics performance, etc.

2024/05/PCB-assembly-for-fine-pitch-of-FPGA-component.webp

Now, we simply discuss the PCB design guideline for a 0.4mm fine pith BGA component to facilitate in PCB manufacturing process.

Standard Guideline Points:

No circuit track allowed between BGA Pads.

2024/05/0.4MM-fine-pitch-BGA-PCB-Design-and-layout-guidelines.webp

Minimum Pad size 0.127mm with 0.1mm laser hole drilled on (this could save much space for PCB layout and reduce final PCB size). And strongly recommend to use stack up: 0.8mm type or 1.2mm type.

2024/05/Laser-drilling-hole-design-for-fine-pith-BGA-PCB.webp

Keep the minimum spacing between track and holes：0.15mm (refer below picture).

2024/05/Clearance-size-design-guidelines-for-fine-pitch-BGA-PCB.webp

Recommend to use Via in PAD design for the plated holes locating in the BGA zone.

Technology Map for 0.4mm Pitch BGA PCB Design

Advanced Technology Limitation for 0.4mm BGA PCB Design

Item Inner layer design without tracks between holes Inner layer design with some tracks between holes Outlayer design without tracks between holes Out-layer design with some tracks between holes
Drill hole size (mil) 6.0 4.0 6.0 Design deed to be exactly evaluated case by case
Track width (mil) 2.00 2.00 /
Spacing between hole and the track (mil) 3.87 4.87 /
Annular ring size per side (mil) / 2.50 3.00
Other notes: PCB thickness<=1.20mm; base copper in inner layers: <=0.5oz PCB thickness<=0.80mm; base copper in inner layers: <=0.5oz PCB thickness<=1.20mm; base copper in out layers: <=0.5oz
1. Can only make prototypes 2. Must be symmetrical stack-up design 3. Layout count <= 6L

1.2 mm Stack-up Guideline (only for 4L):

1.20 mm Stack-up Guideline (only for 4L HDI)

1.2mm thickness stack-up design reference Thickness
L1 Copper 8.5 um
PP 1080
TU-7689
L2 Copper 35 um
Core 900 um
L3 Copper 35 um
TU-7689
PP 1080
L4 Copper 8.5 um
**1 Assumed based copper thickness as 35um in L2 & L3
**2 If copper thickness in L2 & L3 is 17um, the core thickness = 1.0mm
**3 The prepreg PP1080 thickness can be flexibly adjusted
**4 Laser drilling process on L1-L2, L3-L4; the blind hole size 0.1mm

0.8 mm Stack-up Guideline (only for 4L):

0.80 mm Stack-up Guideline (only for 4L HDI)

0.80mm thickness stack-up design reference Thickness
L1 Copper 8.5 um
PP 1080
TU-7689
L2 Copper 35 um
Core 510 um
L3 Copper 35 um
TU-7689
PP 1080
L4 Copper 8.5 um
**1 Assumed based copper thickness as 35um in L2 & L3
**2 The prepreg PP1080 thickness can be flexibly adjusted
**3 Laser drilling process on L1-L2, L3-L4; the blind hole size 0.1mm
2024/05/0.80mm-HDI-PCB-stack-up-design-guidelines-for-fine-pitch-BGA.webp
2024/05/1.20mm-HDI-PCB-stack-up-design-guidelines-for-fine-pitch-BGA.webp

Important Notes to Surface Treatment

Important notes to circuit board surface treatment for 0.4mm fine pitch PCB:

PCB Surface Treatment Design for 0.4mm Fine Pitch Components

Surface finishing Options Rmark
HAL(hot air solder leveling) No-X(the surface is not so smooth so it will take trouble in soldering) ×
HAL Lead free No-X(the surface is not so smooth so it will take trouble in soldering) ×
Immersion gold Good-√ √
2024/05/Gold-finishing-for-PCB-with-fine-pitch-BGA-components.webp

Important notes to PCB solder mask for 0.4mm fine pitch BGA components:

2024/05/Why-using-green-solder-mask-for-PCB-with-0.4mm-fine-pitch-BGA-components.webp

If you need a customized stack-up for 6L (or above) PCB board and have more questions to us, please contact us by service@wellerpcb.com.

Popular posts