Colibri iMX6ULL Design Review and Questions

Hello,
I have designed my own Carrier board for Colibri iMX6ULL computer-on-module. I have used Viola design as reference. You can find the schematics over here. I will be soon sending it to PCB Fab house but I have few doubts that I want to clear before proceeding further.

My questions are:

  1. The Colibri iMX6ULL has seven 3.3V pins. However, viola reference design has only 4 decoupling capacitors? Can someone explain that to me?

  2. Can I add Blinking LED to any pin? Do we have a provision to enable or define a blinking led pin in BSP or in any Software?

  3. I have removed Jumper and resistor R73. I have placed a trace in place of resistor R74 (These designator belong to Viola reference design). Can someone verify my Ethernet design as I want to use only Colibri iMX6ULL board?

  4. I have placed stitching capacitor in my design. I have placed 8 100nF 0603 caps. Any better idea on stitching caps values and placement?

  5. I am not using Resistor Array/bank for SD and SPI interface. I don’t think it will cause any problem as long as length is matched and distance between traces is enough. Am I right?

  6. I have added JTAG connector in my board. I am using Segger Jlink. It’s pinout is over here. You can find the JTAG connector in extension connector page. I have few questions for my JTAG design.

    a. JTAG requires VREF_JTAG. Do I need to connect it to 3.3V?

    b. Colibri iMX6ULL has MOD Pin. It is not required in Segger JLink Connector. What should I do with it?

    c. Segger Jlink has one output pin for System Reset. I have connected it to RESET_EXT#. Is it fine?

    d. I don’t have any series resistor in between JTAG connector and colibri pins. Is it fine?

    e. Segger JLink connector has RTCK pin. However, iMX6ULL doesn’t have such pin. I have grounded that pin. Is it fine?

EDIT

I have few more questions:

  1. During layout and floor planning, I found out SD Card interface lines are of different length. Lines liks CMD and DATA0 are very short. Is this could be problem?

  2. Can I remove resistors to disable PS/2 drivers and resistors to disable CF access (SODIMM PIN 81)?

Hi @abhiarora,

Please read the Colibri design guide and the layout design guide available on our developer website:
https://developer.toradex.com/carrier-board-design/carrier-board-design-guides

Please find the details below:

The Colibri iMX6ULL has seven 3.3V pins. However, viola reference design has only 4 decoupling capacitors? Can someone explain that to me?

The 4 capacitors with specified values are good to provide the instantaneous power required by Colibri module.

Can I add Blinking LED to any pin? Do we have a provision to enable or define a blinking led pin in BSP or in any Software?

No, you can write a small code for blinking LED.

I have removed Jumper and resistor R73. I have placed a trace in place of resistor R74 (These designator belong to Viola reference design). Can someone verify my Ethernet design as I want to use only Colibri iMX6ULL board?

Follow the recommended circuit as adviced you earlier, The current circuit hold good for the Ethernet PHY used on the module. In future, we may have to move to voltage mode PHY on the module, which may require different biasing. If you are not using the recommended assembly, you may have to redesign the section of the board under such situations.

I have placed stitching capacitor in my design. I have placed 8 100nF 0603 caps. Any better idea on stitching caps values and placement?

Why do you need them? Any specific situation where you want to use them? Stitching caps may or may not be required. It is dependent on PCB layout and how you are routing the signals.

I am not using Resistor Array/bank for SD and SPI interface. I don’t think it will cause any problem as long as length is matched and distance between traces is enough. Am I right?

Series resistors are adviced to be used. Length matching is not necessary for SPI or SDIO. Are you sure matching length on carrier board will result in length matched traces for the interface (module + carrier board)?

I have added JTAG connector in my board. I am using Segger Jlink. It’s pinout is over here. You can find the JTAG connector in extension connector page. I have few questions for my JTAG design.
a. JTAG requires VREF_JTAG. Do I need to connect it to 3.3V?

Yes

b. Colibri iMX6ULL has MOD Pin. It is not required in Segger JLink Connector. What should I do with it?

That a strapping signal. The signal is pulled down on the module using a 10K resistor. You can add a header/ Jumper on your carrier board to pull up the signal if you want to enter boundary scan mode.

c. Segger Jlink has one output pin for System Reset. I have connected it to RESET_EXT#. Is it fine?

Since we have not tested it. I would recommend you to add assembly option to connect/disconnect the JLINK reset from the RESET_EXT# signal.

d. I don’t have any series resistor in between JTAG connector and Colibri pins. Is it fine?

Should be fine

e. Segger JLink connector has RTCK pin. However, iMX6ULL doesn’t have such pin. I have grounded that pin. Is it fine?

Leave that pin unconnected OR use 0R resistor series resistor to connect the signal to GND. For more details, refer following article: Documentation – Arm Developer

Regards,
Satyan

@satyan.tx I have read the design guides in the past. Can you comment on Pull-up resistors for disabling PS/2 drivers and Compact Flash Card detect pull-down resistors? Can I remove them?

Regarding Stitching caps, I am changing signal layers for some of the nets. I thought to add caps near to layer switching point.

I have edited my question and added layout related questions. Please help.

During layout and floor planning, I found out SD Card interface lines are of different length. Lines liks CMD and DATA0 are very short. Is this could be problem?

As I told you earlier (in the other community query), SDIO interface don’t length matching on carrier board.

Can I remove resistors to disable PS/2 drivers and resistors to disable CF access (SODIMM PIN 81)?

Leave them unassembled

Hello @satyan.tx,
I am planning to remove them from board to save some space. Can I share my layout files with you so that you can review it?

Hi @abhiarora,

You can remove the resistors for the design.
For layout review, please write to support@toradex.com (Mr. Ritesh Kumar, FAE, Delhi Region).

Regards,
Satyan Raj

Hi @satyan.tx,
Please share your email id too. I will loop you in too for layout.

Hi @abhiarora,

Please write to support@toradex.com, I will be able to follow your queries.

Regards,
Satyan