Minimum PCB Trace width with SMD components and Autorouter problem

Question

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.

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.

Answer 1

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.

Answer 2

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.

Answer 3

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.