Tests Points on a PCB

[ziggyfish]

So,

I have a schematic, and I have my PCB layout done (mostly SMD). However, I would like to add some tests points somewhere on the board for power rails, GND, and other UART, SPI, I2C interfaces.

What is the best way (industry standard way) to do this?

[rx8pilot]

I use a whole variety of options, test points can really save time and frustration.

You can use anything from smd pads, vias with slightly enlarged annular rings, or solder-in hooks that are through hole or smd.

I don't know of any industry standards.

Sent from my horrible mobile....

[AndyC_772]

Use whatever works for you. If it's a board that will likely be tested, serviced or repaired by someone else, then use whatever works for them too.

I tend to:

- put GND points on my PCBs such that nowhere on the board is further away from a GND point than the length of the ground lead on a scope probe. For these I use 1mm drilled holes, into which I can solder short wires as needed. Using a through hole means they're strong enough to support the weight of a few probes, and to survive the odd tug.

- put test points on any nets which I think I might possibly want to probe during the bring-up and testing of a board. These are just circular pads on the top (or bottom) layer, 1mm dia. They just need to be big enough to probe with a scope, or to solder a short wire onto. I use very thin (30AWG) wire to avoid transmitting any significant force to the PCB. Care is needed to ensure the wires don't pull the test pads off the board; I'm completely OK with this, but if you have room and prefer the robustness of a through-hole connection, that makes perfect sense too.

If test points will be used with a bed-of-nails jig, then they need to be far enough apart for the jig to be manufactured. It may be helpful if they're on a regular grid.

I rarely use test point components (posts, hooks and the like). I don't like the rigidity; if a scope probe connected to a fixed test point gets knocked, then there's a danger it'll bend the probe hook or damage the PCB. I much prefer a flexible wire soldered into a hole.

It's most important to put TPs on nets that aren't otherwise accessible. BGA and (arguably) QFN pads are the obvious candidates, plus any net which only exists on the opposite side of the PCB to the one normally exposed.

I generally reckon that any pin on an IC with >0.5mm pitch is fair game for being probed, and so is any passive component 0603 or bigger. Service and repair technicians may beg to differ, so you need to make the trade-off between scattering test points everywhere vs actually fitting all the parts onto the PCB. TPs can take up a surprising amount of space on a dense board, especially if they have to be through holes.

[T3sl4co1l]

I usually use appropriately sized vias, or free pads.

These are tagged as test points (which can be done manually or automatically), and they then appear in the IPC-356 file.

Tim

[plazma]

I made a library of different sizes of round test points.

Sent from my PLK-L01 using Tapatalk

[ziggyfish]

Use whatever works for you. If it's a board that will likely be tested, serviced or repaired by someone else, then use whatever works for them too.

I tend to:

- put GND points on my PCBs such that nowhere on the board is further away from a GND point than the length of the ground lead on a scope probe. For these I use 1mm drilled holes, into which I can solder short wires as needed. Using a through hole means they're strong enough to support the weight of a few probes, and to survive the odd tug.

- put test points on any nets which I think I might possibly want to probe during the bring-up and testing of a board. These are just circular pads on the top (or bottom) layer, 1mm dia. They just need to be big enough to probe with a scope, or to solder a short wire onto. I use very thin (30AWG) wire to avoid transmitting any significant force to the PCB. Care is needed to ensure the wires don't pull the test pads off the board; I'm completely OK with this, but if you have room and prefer the robustness of a through-hole connection, that makes perfect sense too.

If test points will be used with a bed-of-nails jig, then they need to be far enough apart for the jig to be manufactured. It may be helpful if they're on a regular grid.

I rarely use test point components (posts, hooks and the like). I don't like the rigidity; if a scope probe connected to a fixed test point gets knocked, then there's a danger it'll bend the probe hook or damage the PCB. I much prefer a flexible wire soldered into a hole.

It's most important to put TPs on nets that aren't otherwise accessible. BGA and (arguably) QFN pads are the obvious candidates, plus any net which only exists on the opposite side of the PCB to the one normally exposed.

I generally reckon that any pin on an IC with >0.5mm pitch is fair game for being probed, and so is any passive component 0603 or bigger. Service and repair technicians may beg to differ, so you need to make the trade-off between scattering test points everywhere vs actually fitting all the parts onto the PCB. TPs can take up a surprising amount of space on a dense board, especially if they have to be through holes.

It's a prototype (with a fair bit of software to write) so I will do most of the probing. The chips are 0.5mm QFN. And the majority of passive components are 0603 (so they should be fine). There are a couple of 0402s however they are for high-frequency (915Mhz) RF signal filtering (which won't be that useful anyway since my scope is only 200Mhz, 1GPS).

Thanks for your help. Very appreciated.

[bson]

I use Keystone Micro 5015, all it requires is a small pad that can be left unpopulated.

[theatrus]

Use whatever works for you. If it's a board that will likely be tested, serviced or repaired by someone else, then use whatever works for them too.

I tend to:

- put GND points on my PCBs such that nowhere on the board is further away from a GND point than the length of the ground lead on a scope probe. For these I use 1mm drilled holes, into which I can solder short wires as needed. Using a through hole means they're strong enough to support the weight of a few probes, and to survive the odd tug.

- put test points on any nets which I think I might possibly want to probe during the bring-up and testing of a board. These are just circular pads on the top (or bottom) layer, 1mm dia. They just need to be big enough to probe with a scope, or to solder a short wire onto. I use very thin (30AWG) wire to avoid transmitting any significant force to the PCB. Care is needed to ensure the wires don't pull the test pads off the board; I'm completely OK with this, but if you have room and prefer the robustness of a through-hole connection, that makes perfect sense too.

If test points will be used with a bed-of-nails jig, then they need to be far enough apart for the jig to be manufactured. It may be helpful if they're on a regular grid.

I rarely use test point components (posts, hooks and the like). I don't like the rigidity; if a scope probe connected to a fixed test point gets knocked, then there's a danger it'll bend the probe hook or damage the PCB. I much prefer a flexible wire soldered into a hole.

It's most important to put TPs on nets that aren't otherwise accessible. BGA and (arguably) QFN pads are the obvious candidates, plus any net which only exists on the opposite side of the PCB to the one normally exposed.

I generally reckon that any pin on an IC with >0.5mm pitch is fair game for being probed, and so is any passive component 0603 or bigger. Service and repair technicians may beg to differ, so you need to make the trade-off between scattering test points everywhere vs actually fitting all the parts onto the PCB. TPs can take up a surprising amount of space on a dense board, especially if they have to be through holes.

It's a prototype (with a fair bit of software to write) so I will do most of the probing. The chips are 0.5mm QFN. And the majority of passive components are 0603 (so they should be fine). There are a couple of 0402s however they are for high-frequency (915Mhz) RF signal filtering (which won't be that useful anyway since my scope is only 200Mhz, 1GPS).

Thanks for your help. Very appreciated.

For the RF, I generally include a footprint for an SMA or UFL connector selectable with an appropriate series cap if there is an on-board antenna. Without equipment (speca, vna) it's not too useful, but if you're doing PCB antennas it's nice to have a good connection point to both the antenna circuit and the RF side for tuning.

I like to use SMD pads on the bottom side, which is a hold over from when I did this professionally and used a lot of pin probe fixtures. Using a regular grid would allow you to mock up a probe fixture which may be reusable if you really want to go down that route.

[Luminax]

If you're talking about test points, you usually have to also consider :

1) Will you be using automated test?
  or
2) Will you be using semi-automated test?
  or
3) Will you require the points for debug-only purposes

My company, for example, does assembly for remote controls, and all designers put a seemingly 'standard' size pads for tester pin,
which brings us to the next subject : Know what you're going to test it with.
There are through hole pogo-pins, SMD pogo-pins etc etc. Some standards are prevalent in that most of them use a metric size for their test pin shaft/receptacle (S2 for 2mm, S3 for 3mm etc).
Knowing what type of testing jig/equipment you're going to use, and the size of the pin/tip helps picture what type of test points you want to put on your board and might give some room for expansion to the future.

[MagicSmoker]

Another vote for vias as test points. To more easily identify them I make all ground vias square, and label/circle all round vias that are also used as test points.

[Luminax]

That's quite good pre-emptive step I'd say.
Some of the probe tip are designed for the PCB maker's Via bed of nail test so it should serve your purpose well

[T3sl4co1l]

Another vote for vias as test points. To more easily identify them I make all ground vias square, and label/circle all round vias that are also used as test points.

It looks so bizarre, seeing a modern interface (Tag Connect) on a very 80s style layout (square routes, teeny annular rings, square pads).

Only thing missing is the tin plate under soldermask.  I wonder if you can even buy it that way anymore?

Tim

[Rerouter]

Depends a little on what i am using the test pad for (generally breaking out hidden nets)

For stuff that is one off go/no go, its generally a round smd pad on one side of the board, (round so it stands out in a sea of square smd pads)

If its something for debugging and software development i will run a larger square pad with a plated hole the right size for my scope probe tip, if its high speed i'll put 2 closely spaced round plated holes for the ground very close to it for the spring ground clip to poke in to.

If its early prototype that will have a large amount of solder / desolder and modifications made i run a 2x3 rectangle of plated holes with rectangle pads on both sides, so far i havent had any delamination issues with this

[tautech]

I use Keystone Micro 5015, all it requires is a small pad that can be left unpopulated.

Likewise with any of the SMD 0805 test points but much smaller offer trouble for ordinary scope probe and reference clip connection.
Google image of types available:
https://www.google.co.nz/search?q=0805+smd+test+point&rlz=1C1ASUM_enNZ497NZ497&espv=2&tbm=isch&tbo=u&source=univ&sa=X&ei=9fzjU6X1Lpbg8AWk2IDoBQ&ved=0CBoQsAQ&biw=1022&bih=751#facrc=_&imgdii=_&imgrc=IP5iBU8WB1YLuM%253A%3BLDKhSGBicj2eJM%3Bhttps%253A%252F%252Fd2t1xqejof9utc.cloudfront.net%252Fscreenshots%252Fpics%252Fa3009a3531c49e171c8737e9f87e2436%252Fmedium.jpg%3Bhttp%253A%252F%252Fgrabcad.com%252Flibrary%252Ftest-points-smd-1%3B704%3B469

Points like these in 0805 are my favourite when needed:


http://www.nicomatic.com/product-smd_test_terminals-69-en-1-47-334.htm

[Pitrsek]

So,

I have a schematic, and I have my PCB layout done (mostly SMD). However, I would like to add some tests points somewhere on the board for power rails, GND, and other UART, SPI, I2C interfaces.

What is the best way (industry standard way) to do this?

I use silkscreen circled vias and smd test points. Nowadays mostly vias(smaller). For high speed stuff and power supply impedance measurement SMA.
I tend to be test point heavy, probably not 100% coverage, but not far from it. Makes the testing faster, and more enjoyable. Thinking about test-points when layout is done is IMHO too late. I prefer to add test-points as a draw schematics, and then go over it once more when schematics design is closed (that's when I'm thinking about what and how is going to be tested).  Apart from test-points, 0R jumpers and spare pull ups/downs are also handy. So you can test only part of your board when needed.
 

[ziggyfish]

Vias seem like the way to go, considering I already have them in my design.

Thanks, guys/girls.

[MagicSmoker]

It looks so bizarre, seeing a modern interface (Tag Connect) on a very 80s style layout (square routes, teeny annular rings, square pads).

Only thing missing is the tin plate under soldermask.  I wonder if you can even buy it that way anymore?

Tim

If you think my board layout is dated you should see my wardrobe!