Author Topic: PCB routing question  (Read 1933 times)

0 Members and 1 Guest are viewing this topic.

Offline yashrkTopic starter

  • Frequent Contributor
  • **
  • Posts: 268
  • Country: in
  • A MAKER, AN ENGINEER, A HOBBYIST FOR LIFE
    • My Personal Blog
PCB routing question
« on: August 16, 2018, 12:23:46 pm »
Hey guys,

I am working on an office project where we are using multiple SPI ICs on a single bus and as the orientation and pins of the IC is fixed I had to route the bus in the manner shown in the image. I am tapping these signal where there is an IC connected as shown in the image. The bus spans 310 mm long where the signals from the controller are inserted in the middle. SPI clock will be at <10MHz. the board is two-sided and has a ground flood fill in between them.

Sorry I cannot share the whole layout as its an office project.

1. I am concerned that the clock line going over the other lines may cause a problem, what are your views on that?

2. Is there anything else I need to take care about considering the length of the bus?  i.e. 310mm/2 = 155mm on either side

Thank you,
Yash.
Find me and things I'm working on - https://www.yashkudale.com/
 

Offline T3sl4co1l

  • Super Contributor
  • ***
  • Posts: 21606
  • Country: us
  • Expert, Analog Electronics, PCB Layout, EMC
    • Seven Transistor Labs
Re: PCB routing question
« Reply #1 on: August 16, 2018, 09:06:10 pm »
Stubs this short are only a concern with high speed interfaces, not SPI.

The angled bits could stand to go, they just look ugly (some will call the acute angles acid traps, but that apparently isn't a problem anymore; so I stick with an aesthetic reason instead).

Add stitching vias around the bus.

If you want, add source termination resistors, at each driving pin (so, at master SCK, MOSI and CS's, and at slave MISO's).  47 ohms would be typical, or higher if you don't need super fast operation.

Tim
Seven Transistor Labs, LLC
Electronic design, from concept to prototype.
Bringing a project to life?  Send me a message!
 
The following users thanked this post: yashrk

Offline Deridex

  • Regular Contributor
  • *
  • Posts: 166
  • Country: 00
  • IMHO
Re: PCB routing question
« Reply #2 on: August 17, 2018, 03:41:01 am »
I don't think that you need to worry about the SPI bus in therms of routing this way.
For me it looks like the SPI has only little requirements to the routing. The only problem i remember so far, was with very fast rise&fall-times that were adjusted with a resisitor.
 
The following users thanked this post: yashrk

Offline yashrkTopic starter

  • Frequent Contributor
  • **
  • Posts: 268
  • Country: in
  • A MAKER, AN ENGINEER, A HOBBYIST FOR LIFE
    • My Personal Blog
Re: PCB routing question
« Reply #3 on: August 17, 2018, 06:05:54 am »
Stubs this short are only a concern with high speed interfaces, not SPI.

The angled bits could stand to go, they just look ugly (some will call the acute angles acid traps, but that apparently isn't a problem anymore; so I stick with an aesthetic reason instead).

Add stitching vias around the bus.

If you want, add source termination resistors, at each driving pin (so, at master SCK, MOSI and CS's, and at slave MISO's).  47 ohms would be typical, or higher if you don't need super fast operation.

Tim

Thanx for your comment, I have 47ohm resistors in series with each and every pin near the slave side as well as the master side I will then just populate the resistor on the master side, MISO on the slave side and will put a 0ohm resistor on the remaining pins. Or is it better to have 47ohm resistors on both sides?

Regards,
Yash
Find me and things I'm working on - https://www.yashkudale.com/
 

Offline T3sl4co1l

  • Super Contributor
  • ***
  • Posts: 21606
  • Country: us
  • Expert, Analog Electronics, PCB Layout, EMC
    • Seven Transistor Labs
Re: PCB routing question
« Reply #4 on: August 17, 2018, 07:14:28 am »
Yeah, that'll be fine, the 47 and 0's. :)

Tim
Seven Transistor Labs, LLC
Electronic design, from concept to prototype.
Bringing a project to life?  Send me a message!
 
The following users thanked this post: yashrk

Offline Mattylad

  • Regular Contributor
  • *
  • Posts: 143
  • Country: gb
Re: PCB routing question
« Reply #5 on: August 26, 2018, 10:54:24 am »
Every time I have been to a pcb fab house this century - they have confirmed that acid traps ARE still a problem, just not as big as it used to be so it is still good practise to reduce as much as possible all angles of less than 90 degrees, such as those pictured in the Op.
Matty
CID+
 

Offline yashrkTopic starter

  • Frequent Contributor
  • **
  • Posts: 268
  • Country: in
  • A MAKER, AN ENGINEER, A HOBBYIST FOR LIFE
    • My Personal Blog
Re: PCB routing question
« Reply #6 on: August 27, 2018, 04:14:26 am »
Every time I have been to a pcb fab house this century - they have confirmed that acid traps ARE still a problem, just not as big as it used to be so it is still good practise to reduce as much as possible all angles of less than 90 degrees, such as those pictured in the Op.

Yeah, I fixed that.  :-+
Find me and things I'm working on - https://www.yashkudale.com/
 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf