AM263P4-Q1: PCB Stack up design

Hi Amit,

Have you reviewed our HW design guideline document before? This is the best resource we have: https://www.ti.com/lit/pdf/sprabj8

Any constraints would be highlighted in it.

If you have specific questions, I can have one of our HW experts provide some comments.

Best Regards,

Ralph Jacobi

Hi Amit,

Adding on to what Ralph said above, please do review the Hardware Design guideline what Ralph pointed out above.

Most of our EVMs(like PROC159E2) are designed to demonstrate multiple peripherals on the same board for easier evaluation. For this a lot of on-board Mux and De-Mux are used. One starting point would be to start planning with which peripherals to use using Sysconfig and then remove these un-used Muxed peripherals based on your use case. This would greatly reduce the complexity of the board and especially the fanout. Few quick things with respect to PROC159E2 I can think of are below

1. Since you are using AM263P4 with Flash in Package variant, you would not need both the OSPI and QSPI peripherals and their mux. This would greatly help with fanout.
2. If your application does not use HSEC connector of PROC159E2, it will greatly reduce the routing complexity.
3. Multiple muxes for I2C, UART, JTAG, ICSS might not be needed based on use case. Most of then are used for the HSEC edge connector.
4. GPIO Expander might not be needed in all use cases since above changes would free up some GPIOs
5. All ADCs and their Mux might not be used.

Few or all of the above should help you reduce the layer count of the board.

Thanks,
Tejas Kulakarni

Hello Amit,

Sure, these are hosted on our tool pages for the devices.

The LP-AM263P design files can be downloaded from: https://www.ti.com/lit/zip/sprr503

The AM263P controlCard (PROC159A) files can be be downloaded from: https://www.ti.com/lit/zip/sprr492

Note that the PROC159E2 was a pre-production release and PROC159A is the production release which is why there is a difference in the E2 vs A nomenclature.

Best Regards,

Ralph Jacobi

Amit, 

Neither of the above is necessarily mandatory when designing a PCB system with AM26x devices. However, it is strongly suggested to follow what has been outlined in the Hardware Design Guidelines document. The document reflects what has been implemented and proven to function properly on TI Evaluation Boards. By straying from what TI recommends, you assume the risk of improper operation of the AM26x device on your PCB system.

Regards,

Brennan

Hey Amit,

Both the variants of PTH and PTH via in pad are used in different boards as per their application and routing needs. PTH or PTH via in pad can be used as per the needs of the application. More dense applications can use PTH via in pad, less dense applications can use plain PTH. The same is explained in Section 11 Vias of https://www.ti.com/lit/an/sprabj8b/sprabj8b.pdf with respect to our EVMs.

Amit Teke said:

possible to use 0402 decoupling capacitor under BGA

Based on the via size used in our EVMs it is not feasible to place 0402 decoupling capacitors under the BGA(BGA on top layer and decap on bottom layer). We have relied on using 0201 decaps under the BGA.

Thanks,
Tejas Kulakarni

Hi Amit,

Amit Teke said:

1) Which type of via used in this board?  Type VII?

There are multiple types of vias used. But if you are interested in the resin filled and cap plated vias, yes IPC 4761, Type VII vias are used. More details can be referred from: Fabrication Note 17 in PROC159A_FAB.pdf inside the design files of TMDSCNCD263P.

We will come back to you on the Via in Pad usage for fan out.

Thanks,
Tejas Kulakarni

Hi Amit,

Via-in-pad construction is used on some ICs with a thermal pad (for example, U84, U85, etc) on the AM263Px control card EVM.

For the AM263/Px BGA fan-out itself, via-in-pad is not used.

Regards,

Brennan

Amit,

Correct, the Hardware Design Guidelines document is incorrect and will be updated for the next revision.

The vias on the thermal pad are technically via-in-pad construction but are not resin filled & cap plated.

Regards,

Brennan

Amit,

Correct, there is no requirement for via-in-pad under the AM263Px BGA. You can certainly do it if you want, but it is not a design requirement.

Regards,

Brennan

Amit,

Once a thread has been resolved by the original poster, it is better to start a new thread for organizational purposes.

I will answer here for convenience, but just for future reference  

L4 and L7 GND layers are used to aid power integrity and EMI, since power is routed on L5 and L6. High-speed traces are routed on L3 and L8, between respective GND planes L2 and L9.

Regards,

Brennan

Amit,

The AM26x LaunchPads are the low-cost evaluation platform for the AM26x devices. They are more optimized than the control cards in order to reduce cost and represent an inexpensive AM26x PCB solution for designers to base their systems off of. The LaunchPads have less hardware/external interfaces than the control cards, which influences the # of signals that need to be routed, and thus, the # of PCB layers.

On the LaunchPads, high-speed signals are routed on layer 3. The majority of the power is routed on layer 4. Layer 5 is the GND for the L4 power, and Layer 2 is the GND for L3 signal routing.

Regards,

Brennan