Author Topic: Routing test traces next to PCB edge - bad idea?  (Read 738 times)

0 Members and 1 Guest are viewing this topic.

Offline simonlasnier

  • Frequent Contributor
  • **
  • Posts: 251
  • Country: dk
Routing test traces next to PCB edge - bad idea?
« on: April 08, 2021, 02:19:11 pm »
Hi :)

Just wondering - I know routing traces next to the PCB edge is a bad idea for EMC as they might couple with the metal case.

But what would it be ok if these traces are used to get to a test connector, only used while testing the board? I am thinking under normal operations (i.e. not under test) there should not be any current flowing in those traces, then it does not matter they are next to the edge of the PCB?

Thank you

Simon
 

Offline elecman14

  • Supporter
  • ****
  • Posts: 163
  • Country: us
Re: Routing test traces next to PCB edge - bad idea?
« Reply #1 on: April 08, 2021, 02:45:23 pm »
You would also want to consider ESD.  Depending on how exposed it is you may have a return path to whatever you are testing.
 

Offline fourfathom

  • Frequent Contributor
  • **
  • Posts: 678
  • Country: us
Re: Routing test traces next to PCB edge - bad idea?
« Reply #2 on: April 08, 2021, 02:56:13 pm »
But what would it be ok if these traces are used to get to a test connector, only used while testing the board? I am thinking under normal operations (i.e. not under test) there should not be any current flowing in those traces, then it does not matter they are next to the edge of the PCB?

Current always flows in a trace, on signal transitions, even if there is no load connected at the end.  It's still a transmission line.
 

Offline simonlasnier

  • Frequent Contributor
  • **
  • Posts: 251
  • Country: dk
Re: Routing test traces next to PCB edge - bad idea?
« Reply #3 on: April 08, 2021, 06:05:19 pm »
Thank you for the replies.

@elecman14: the test will be done in a ESD controlled environment so that's ok.

@fourfathom: kinda what I was fearing - just to make sure I get it, here is an example with one of my test traces:

Code: [Select]
DAC output -> OpAmp -> trace -> audio connector
                             ^-> trace along edge -> test connector

Yes one of my test traces is actually an audio signal - it is a headphones output though so I am not worried about the noise (it will need a sufficient amount before you can hear it). The other test traces are a mix of digital inputs and outputs (everything under 50kHz and with soft edges)

But back on what you said, if current flows from the opamp output to a pair of headphones, and nothing is connected on the test connector, most (all?) of the electrons will take the path of least resistance/impedance, which is the direct trace between Opamp and the audio connector, and not go through the trace along the edge, or did I get that wrong?

Thank you!
 

Offline fourfathom

  • Frequent Contributor
  • **
  • Posts: 678
  • Country: us
Re: Routing test traces next to PCB edge - bad idea?
« Reply #4 on: April 08, 2021, 09:52:27 pm »
The other test traces are a mix of digital inputs and outputs (everything under 50kHz and with soft edges)

But back on what you said, if current flows from the opamp output to a pair of headphones, and nothing is connected on the test connector, most (all?) of the electrons will take the path of least resistance/impedance, which is the direct trace between Opamp and the audio connector, and not go through the trace along the edge, or did I get that wrong?

You got it right.  At audio frequencies the current will be flowing to the load, and an open trace will see virtually no current.

For audio and other soft-edge signals the transmission line effects will be pretty microscopic and I wouldn't worry about it.  As you mentioned, there still is a chance your signals will pick up crosstalk from adjacent traces, so keep any close parallel sections to a minimum.  You can add a grounded trace between source and victim traces to reduce capacitive coupling, but this is seldom necessary with reasonable layout.
 

Offline simonlasnier

  • Frequent Contributor
  • **
  • Posts: 251
  • Country: dk
Re: Routing test traces next to PCB edge - bad idea?
« Reply #5 on: April 09, 2021, 03:24:43 pm »
Ok thank you fourfathom :)
What about high frequency signals, will there be current in the test traces then?

One of my digital signal is 35kHz, but because of the edges probably has frequencies around 1-10MHz - I'll make sure to keep that one away from the edges!
 

Offline fourfathom

  • Frequent Contributor
  • **
  • Posts: 678
  • Country: us
Re: Routing test traces next to PCB edge - bad idea?
« Reply #6 on: April 09, 2021, 04:06:24 pm »
What about high frequency signals, will there be current in the test traces then?

One of my digital signal is 35kHz, but because of the edges probably has frequencies around 1-10MHz - I'll make sure to keep that one away from the edges!

There will be a small amount of current in the unterminated test traces.  Since at 10 MHz the traces are probably too short to be usefully analyzed as a transmission line (but you can), just consider the trace capacitance.  This capacitance will be charged and discharged during the clock transitions, and this results in current flowing through the trace.

As far as coupling to a metal case, with your conditions it seems like a very minor factor.
 

Offline Terry Bites

  • Frequent Contributor
  • **
  • Posts: 355
  • Country: gb
  • Recovering Electrical Engineer
Re: Routing test traces next to PCB edge - bad idea?
« Reply #7 on: April 09, 2021, 05:33:52 pm »
Use a ground-plane to stop stuff spilling of the edge of your board. Groundplanes are good for the planet, less toxic Cu down the drain.
 

Offline simonlasnier

  • Frequent Contributor
  • **
  • Posts: 251
  • Country: dk
Re: Routing test traces next to PCB edge - bad idea?
« Reply #8 on: April 10, 2021, 12:52:24 pm »
Ha ha good plan :D
It's a two layer board and of course both layers have a ground pour on them.

But that one audio trace is actually close to the egde so that there is no ground copper between the trace and the edge.
 

Offline fourfathom

  • Frequent Contributor
  • **
  • Posts: 678
  • Country: us
Re: Routing test traces next to PCB edge - bad idea?
« Reply #9 on: April 10, 2021, 07:15:58 pm »
That audio trace *is* over a groundplane, and in most cases that's more effective than adjacent ground traces.
 

Offline JustMeHere

  • Frequent Contributor
  • **
  • Posts: 412
  • Country: us
Re: Routing test traces next to PCB edge - bad idea?
« Reply #10 on: April 10, 2021, 08:06:26 pm »
Ha ha good plan :D
It's a two layer board and of course both layers have a ground pour on them.

But that one audio trace is actually close to the egde so that there is no grounFCCd copper between the trace and the edge.

4 layer boards are cheap these days.
 

Offline simonlasnier

  • Frequent Contributor
  • **
  • Posts: 251
  • Country: dk
Re: Routing test traces next to PCB edge - bad idea?
« Reply #11 on: April 12, 2021, 08:52:25 am »
Ok thanks :)

And yes 4-layer boards are cheap - but if I do not need it why would I bother :)
 

Offline fcb

  • Super Contributor
  • ***
  • Posts: 1958
  • Country: gb
  • Test instrument designer/maker G1YWC.
    • Electron Plus
Re: Routing test traces next to PCB edge - bad idea?
« Reply #12 on: April 12, 2021, 09:49:26 am »
Unlikely to have any EMC implications if it's audio.

If it connects straight to a headphone jack then it's likely ESD protected???  So no worries there for ESD discharge testing.

*New Product - 5V TC reference* available now.
https://electron.plus Power Analysers, VI Signature Testers, Voltage References.
 

Offline JustMeHere

  • Frequent Contributor
  • **
  • Posts: 412
  • Country: us
Re: Routing test traces next to PCB edge - bad idea?
« Reply #13 on: April 12, 2021, 06:02:07 pm »
Ok thanks :)

And yes 4-layer boards are cheap - but if I do not need it why would I bother :)

Having a big solid ground pane under all of.your signals eliminates all sorts of noise.

Your inner two layers should be solid as possible.  (Make sure your holes have some copper between them.)  These give you an easy place to route power.  That gives more options for routing signals.

I think there's a company charging the same price for 4 layers as 2 layers
 

Offline TheHolyHorse

  • Regular Contributor
  • *
  • Posts: 178
  • Country: se
  • You don't need to be confused, just understand it.
Re: Routing test traces next to PCB edge - bad idea?
« Reply #14 on: April 13, 2021, 08:51:54 am »
I think there's a company charging the same price for 4 layers as 2 layers

Who would that be? And what is their price of 2 layer boards  ;)
 

Offline tautech

  • Super Contributor
  • ***
  • Posts: 21471
  • Country: nz
  • Taupaki Technologies Ltd. NZ Siglent Distributor
    • Taupaki Technologies Ltd.
Re: Routing test traces next to PCB edge - bad idea?
« Reply #15 on: April 13, 2021, 11:22:14 pm »
If you need PCB test points for other than bed of nails testing like prototyping just use SMD test points where you just lay down a SMD footprint directly on a net/trace and assign both pads of the footprint to the same net.
No need to break out test point traces to the PCB edge.
Then solder them on like any SMD device where you can connect to them with grabbers or scope probes for your measurements. Don't forget to add one on the ground plane for a reference point.  ;)
If you need to ID each test point just add some text as copper or into the overlay.

The process of using these should be an early part of your PCB layout so to have room to connect to them and also provide room for the ID text.



Most suppliers stock a few brands and styles of these but I like the style above from Keystone.
Easy to use, remove and reuse.
https://www.keyelco.com/category.cfm/keyelco/Test-Points-Tips-Probes-Clips/id/518
Avid Rabid Hobbyist
 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf