PCB trace Width/Space

[Falcon69]

Working on another circuit board. But I have a question...

Below is a picture of a couple of 0402 resistor footprints.

The trace width is 6mil (per most manufacture recommendations) and the space between the trace and the resistor is 6mil equally.

There will be no more than a total of 100mA flowing through the trace and/or resistors.

If I design the board with this type of spacing between parts and other traces....what are some things I need to be aware of? Like for example, power jumping over tracks and messing with the operation of the circuit?

Now, the only board I have to look at with spacing/traces smaller then that is an old computer motherboard I have. It looks like the spacing they have is 3mil in some parts. That's pretty small. I'd love to be able to design down that small, but then I'd have to do a premium service to manufacture the boards, and, like above, I don't know what the problems that could arise from doing so when making trace/widths that low.

So, is it safe to design the board as in the picture with 6mil space/trace width between other traces and components?

The only rule I know of so far (still learning) is between large power traces (i.e. large amounts of Amps) the spacing should be large between the trace and other traces/components.

Also, I have a trace drawn under the 0402 resistor, same spacing/trace width. Okay?

[Falcon69]

nobody has designed a board this way?

If so, have a pic of the 0402's with a trace next to and below it?

[exmadscientist]

nobody has designed a board this way?

Nobody in the last hour, anyway... patience is a virtue, they tell me.

This will be fine from an assembly point of view. Soldermask will prevent anything from shorting where it shouldn't.

From a design point of view, it depends entirely on the circuit. If these are all non-critical circuit nodes, it should be fine. If this is a critical section of an analog circuit that is sensitive to leakage, then I would not do this.

[Falcon69]

what do you mean by leakage?

it's just caps, leds, resistors, and logic gates....pretty much all the circuit is.

[kuromaku]

Those look like stock Diptrace land patterns... if so, watch out for tombstoning of the parts.

It'll most likely work for a hand-built one-off with the traces like that, but with soldermask swell you might not have enough mask web to guarantee cleanliness, depending on the fab house.

I would come up with your own land patterns closer to 7351B (which will be smaller than the stock Diptrace ones) and try to not route the traces that way if possible.

[T3sl4co1l]

Yes but.....

Referring to e.g. http://www.vishay.com/docs/20035/dcrcwe3.pdf
the 0402 part is max 1.05 x 0.55 (L x W) mm.  Min length 0.95mm.  Maximum electrode (T1) of 0.30mm, which means a minimum gap (L(min) - 2 * T1(max)) of 0.95 - 0.6 = 0.35mm.

IPC (nominal / level B density) recommends +0.1 toe, -0.05 heel and +0.0 side.  So the pads should be total length 1.25mm ('Z' dimension), gap of 0.40mm ('G'), and width ('X') of 0.55mm.  (Which means pads of 0.55 x 0.425mm at +/- 0.825 mm centers.)

6 mils is 0.15mm (more or less), so 6 mils trace + 2 space is 0.45mm, which is just too tight to fit within 'G'.  (More exactly, 18 mils is the total track + clearance required, and you have 15.75 mils.)

If these are the dimensions of your footprint, then congratulations, you have an IPC compliant footprint!  But, you won't be able to do what you show above.

There's also the consideration of solder mask.

Solder mask alignment is typically 3 mils in any direction.

Minimum web width is typically also 3 mils.  We don't have to worry about that here (0.4mm - 2 * 0.075mm = 0.25mm, which is > 0.15mm).

There's also a mask-opening-to-metal clearance to beware of: copper that's supposed to be covered in mask, should have 3 mils of soldermask around it as well, so that the soldermask has a chance to stick to the PCB.

If you place traces as close as possible to the edges of a square pad, the corner of the soldermask opening will be sqrt(2) * 3 mils out from the corner of the pad.  Subtract that from 6 and you have less than 3 mils of soldermask around that trace.

At least in Altium, setting the pads as rounded rectangle (with a nonzero corner radius) changes the mask opening to a rounded rectangle as well (as it should be), so mask and copper clearances will come out okay.

So with square pads, the also square route you show would be okay (if clearance is okay).

Tim

[Falcon69]

thank you teslacoil.

I just looked at that vishay data sheet, all dimensions of those resistor pads are what the vishay says for pad dimensions for the 0402.

so if i stick to those dimensions, there's not enough room to do this?

I'm alittle confused on your explanation.

If my pad is .55mm wide, and i have a trace ~6mil spaced off of it, that leaves ~3mil soldermask sticking to the PCB from the trace and ~3mil of non soldermask around the pad.

so, between the pads, according to the vishay data sheet you linked....i need .45mm between the pads, but the pad dimensions call for .5mm spacing (which I have drawn the pads as, exacrtly to those dimensions) between the two pads, so there IS enough to do as I have drawn...yes?

But, if I understand your explanation, about the rounded solder mask and square corners, i'm okay, but if I round that inside corner of the Trace (not the pad), then there won't be enough (since DipTrace does not have that option as Altium does about round corner soldermask).  Like if I did it like this......

[T3sl4co1l]

Yeah, you wouldn't be able to buttress the inside corners.  Which isn't really a problem, just kind of ugly.  It's annoying if you have a single trace (rather than a tee) that's making an "S" shape as it crosses under the part (45 degree corners are nice).

I don't really care about pad width because positioning the parts is a free variable (unless you have reasons).  The copper limited spacing would be parts spaced on 1mm centers.



Showing violation distances (IPC compliant footprint, 6 mil trace) and part-to-part distance (a hair over 1mm).

Note that the courtyards (green) overlap, so these parts are awfully close together.  Most assemblers suggest 50 mil part-to-part clearance (for exposed-termination SMTs like this) for easy assembly and rework.

Tim

[Falcon69]

okay, I should be good then, as long as I stay with the dimensions or greater than i have now.  Thank You Teslacoil.

Now, the next question.....Do I have anything to worry about using the components i mentioned above with running the traces that close?

[tszaboo]

I'm generally not comfortable putting traces under 0603. The PCB manufacturer uses NSMD, non solder mask defined pad, in this case. Which means there will be a solder mask opening around the pad. I dont think it is sci-fi to see that the track will not be fully covered by the mask, i've seen shift between the mask and the copper.

[T3sl4co1l]

As long as the clearance rule is obeyed, the PCB will be fine.  The extra pad gap required may make tombstoning an issue for assembly, though.

Also, have you considered resistor arrays?  Not always the solution, but can be handy sometimes.

NANDBlog: I discussed soldermask clearances above

Tim

[Richard Head]

So that's what T3sl4co1l means! Teslacoil. I never got it.

[tggzzz]

what do you mean by leakage?

it's just caps, leds, resistors, and logic gates....pretty much all the circuit is.

A capacitor is "formed" when two conductors are proximate to each other. If unintentional, then it is often termed parasitic capacitance.
An inductor is "formed" when current flows through a conductor. If unintentional, it is often termed parasitic inductance.
A resistor is "formed" when current flows between two points. If unintentional it is often termed leakage resistance.

All of those happen all the time, can all be non-linear (especially resistance), and are one of the reasons RF is regarded as a "black art".

[T3sl4co1l]

So that's what T3sl4co1l means! Teslacoil. I never got it.

I've been using this name or a slight variation since about 2000, but the awareness of... the type of substitution used, seems to have faded quickly after 2005 or thereabouts.  Kids these days are just missing out on everything... And, I suppose, it works the same backwards too, if you're much older.

Tim