1
\$\begingroup\$

I would like to receive some suggestions from you about the trace width for my PCB. I'm using some SMD components (ATmega328p TQFP32 and FT232), the main power is 5VDC at maximum 2A. I use also a ESP Wi-Fi module, but the maximum current comsumption will be lower than 2A for sure.

My PCB manufacturer says that the minimum trace width should be 16 mils with copper thickness 105um.

I used an online calculator and it recommends to use a width of 7 mil for the external traces on the PCB (my PCB will use only two layers).

So, it is OK to set 16 mils for the traces?

Thank you and sorry if the question looks too much stupid.

enter image description here

This is the result of the Eagle autorouter and as it is possible to see the problem is with the SMD components. I think it's because the traces are still too wide for the SMD components pins.

enter image description here

\$\endgroup\$
  • \$\begingroup\$ Why 105 um copper? That's 3x the usual value. \$\endgroup\$ – The Photon Jun 7 '18 at 14:45
  • \$\begingroup\$ Because there is a part on my PCB which uses higher power and so I need 105um. \$\endgroup\$ – Marcus Barnet Jun 7 '18 at 15:03
  • \$\begingroup\$ What factors went into the 7 mil reccomendation? \$\endgroup\$ – The Photon Jun 7 '18 at 15:19
  • 1
    \$\begingroup\$ That layout is horrific. Don't use the autorouter. Do it by hand - it'll turn out so much better. Autorouters are only for experts who know how to properly set up ALL of the required rules. They are not designed for beginners who don't know how to route a board. \$\endgroup\$ – DerStrom8 Jun 7 '18 at 16:46
  • 1
    \$\begingroup\$ The routing is very inefficient. There's lots of looping, empty area, useless copper, acute angles, wasted space, etc. Nothing about the routing is logical. Keep connections as short as possible, eliminate loops and dead copper, and empty space where the pour doesn't fill. \$\endgroup\$ – DerStrom8 Jun 7 '18 at 17:52
1
\$\begingroup\$

The 7 mil reccomendation is a minimum to avoid excess heating from a 2 A current. A wider trace is no problem.

The challenge will be making footprints for your fairly fine-pitch SMD parts that can be manufactured with your heavy copper requirement.

\$\endgroup\$
  • \$\begingroup\$ Infact, as you say, I'm having hard time to make the Eagle autorouter complete the routing. It always stops at 82% and get stuck. There are some nets on the SMD components which give problems. I'm adding a picture of my PCB. \$\endgroup\$ – Marcus Barnet Jun 7 '18 at 15:37
1
\$\begingroup\$

The requirements are usually not set by your PCB manufacturer they are set by you.

Two problems arise when traces are small:

1) More resistance, this causes power loss, it also 'creates' a resistor that was not on your schematic which can cause unintended operation. Make sure the resistance will not be a problem for your design (as small as it may be)

2) Self heating from power loss, while related to resistance, extra heat on your board may create a problem for components or even your board. If the temperature rise is too high (~100C) it can cause delamination of the layers. Tens of degrees higher then that and the board will start to burn. Make sure your power loss is not going to cause a destructive temperature rise.

The second thing to consider is how long will you be drawing the 2A of power, is it a max current rating or an average power rating, if it only draws 2A for 1s every minute or so, your average power will lower and can be considered differently in a temperature rise situation. If it draws 2A all the time then you would size the trace larger.

The other thing to consider is board size, if you have lots of room, make the traces bigger and don't worry about the calculations. If your board size really is a limiting factor, then go to a higher weight of copper which makes the traces taller and cuts back on resistance.

As far as the SMT pads go, they are what they are, and they are sized appropriately. You can run bigger traces into a smaller pad to cut back on resistance, realize that more copper around a pad can make it harder to solder because it wicks heat away from the part when soldering which can make it harder to hand prototype.

\$\endgroup\$
  • \$\begingroup\$ The system will never draw 2A, I specified 2A just because the power supply can provide up to 2A. The system will draw at max 1A in the worst case. \$\endgroup\$ – Marcus Barnet Jun 7 '18 at 15:40
  • \$\begingroup\$ Then size it for 1A, the numbers are just an example \$\endgroup\$ – Voltage Spike Jun 7 '18 at 15:40
  • \$\begingroup\$ I set 2A in the online calcualtor to be sure to oversize the system just for safety purposes. Sorry, I didn't mentioned it. \$\endgroup\$ – Marcus Barnet Jun 7 '18 at 15:42
1
\$\begingroup\$

You can always use a wider trace, provided it's possible to make the footprints and spacing that is required for your parts and layout. Probably they also want the spaces to be 16 mils, or maybe a bit tighter is possible depending on how their etch process works.

That's a bit coarse- your TQFP-32 has 0.8mm pitch pins (assuming that's the tightest pitch part) so your track width and space should be better than 15.7 mils just to get to the package, the optimum pad width might be a bit different (my IPC-compliant generator says 0.55mm wide, which is 21.6 mils, so the space will be less than 10 mils). Check with your supplier that the space is okay.

The main problem is that when you specify very thick copper (3-oz = 105um is relatively thick) the etching process limits how narrow the traces can be and how narrow the spaces can be because of undercutting or non-orthogonal etching.

You could also find a better supplier- one I've used allows (for 3-oz Cu) 10 mil tracks and spaces which is (just) okay, or go to the more common 2-oz or 1-oz copper and widen your power traces. You'll definitely save a fair bit of money and have more choices.

\$\endgroup\$
  • \$\begingroup\$ Thank you for the support. I'm trying to figure out how to solve the problem with the routing since at the moment the Eagle autorouter is not able to complete the process. I tried to run a test with a lower trace width but the result is the same. \$\endgroup\$ – Marcus Barnet Jun 7 '18 at 15:41
  • 1
    \$\begingroup\$ How much lower a trace width? Can you experiment with a simpler schematic to test that? \$\endgroup\$ – mike65535 Jun 7 '18 at 16:05
  • 1
    \$\begingroup\$ Consider using hand routing exclusively. It will give you a better layout and a better feel for placement. \$\endgroup\$ – Spehro Pefhany Jun 7 '18 at 16:27
  • \$\begingroup\$ I tried to lower the trace width to 10 mil and the autorouter stops at 92% instead of 83%, but still can't complete the process. I would like to try the manual routing, but I'm not very good to do it manually. \$\endgroup\$ – Marcus Barnet Jun 7 '18 at 16:45

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.