Looking For Feedback On My First PCB Layout

[Efe_114]

Below is a PCB layout I made of a relaxation oscillator, and I'm curious if there is anything I can improve about it. It would be great if you could provide some learning material on PCB design. Also sorry if this doesn't belong in Projects/Designs.

[ataradov]

Having schematics when reviewing PCB layout provides a much better idea of whether layout good or bad.

LMH6609 does not have a thermal pad, and removing it from the footprint would let you route things much cleaner. Also LMH6609 has absolute maximum supply voltage +/-6.6V.

There is no reason for R3 to be rotated 45 degrees. It only makes things worse.

Given the connector you use, your PCB would have to be double sided, so you might as well use that to route power supplies and keep the top layer for the signals.

[Efe_114]

LMH6609 is not the part I will be using, I just chose that part for the foorprint, not to mention I completely forgot about 2 layers    . Is there a specific reason why rotating a part 45 degrees is bad? or is it just bad in this particular case? Also I'm attaching the schematics. Thank you for your help!

[ataradov]

You can still set the correct value for the part. It avoids confusion. Plus I doubt generic opamps would have an exposed pad, so you can at least pick the correct footprint. It will simplify your routing.

Running traces under the parts is also not a great idea. It is possible, but if you can avoid it, you should. And once you move power supply to the other layer, it would be way easier to do.

If you are assembling by hand, 45 degree parts are just more annoying. For a single board it does not matter, by why make the design worse for no reason?

And for C2, it is better to have two capacitors - one for negative and one for positive rail.

After you clean up the routing and placement, I would increase the trace width. There is no reason to go with narrow traces when you have plenty of space.

[MarkF]

Personally, I avoid running traces underneath SMD resistors and capacitors let alone trying to run two traces.  The tolerances are just too tight.
You might get away with it on 1206 or bigger footprints.  But, why?

I also don't run traces at 45^o on the inside corners of those pads.
Unless you are really tight on space, why push the limits and risk shorts?

[Infraviolet]

If this was my first design, and I was going to hand assemble it (either with paste or with using regular solder and delicate work with an iron) I'd be putting R2 and C2 further out from the IC's legs, make it easier to get at the IC legs if I needed to rework them. Once one is more experienced bringing them this close is fine.

I'd also use silkscreen to put markers on each of your input pin pads, so on the real board you can instantly see which is which for when probing it.

And I'd either put a star mark in silkscreen near pin 1 of the IC, or some curve marks near whichever end of the chip has that little semicircle depression, or both, to make it absolutely obvious which way round I put the chip when soldering.

And, although this will be controversial, I'd avoid that very sharp acute angle between traces where they come together under C2. I'd try to have that merger of lines be at 90 degrees or an obtuse angle. Acute angles used to, although there is less risk with modern production processes, serve as acid traps which could result in traces being dissolved during manufacture. Some people say not to even let 90 degree angle exist, always go to >90, but 90 is usually fine. Have the line to the connector merge perhaps at the place where the other branch of this trace has the next corner (the one by the top right of the 2 of C2.), it can easily do a 90 degree or obtuse at this point.

[Doctorandus_P]

Like Infraviolet, I would place R2 and C2 further away from the IC for easier soldering.

And what's this "Earth"? (even though only a single resistor is connected to it)
You  can probably remove it altogether by using a voltage divider on your power supply, but that's not my main concern.

"Earth" is usually used for a mains safety earth, and this is different from "Ground" which is a common name for the voltage level which is used as a "Zero volt" reference.

As you have plenty of room:
I usually add a test pin or similar to the GND connection to easily add the GND clip of my oscilloscope.

And for the dual layer...
PCB manufacturers that doe single layer PCB's cheaper then double layer PCB's are becoming rare. The single most important feature for the other layer is to be a single continuous GND plane. These days lot's of PCB's are routed on 4 layers, even though they could be done on two layers. But with 2 layers you can't make a continous GND plane anymore, or stitching a half decent GND plane together from pieces on top and bottom is very cumbersome and time consuming (and still second rate).

When PCB's become more complex (and have fast logic) GND planes become very important. Some guy at Altium has made a two hour video about GND planes, and all two hours are worth watching. (and studying, and applying to your own designs).

[mariush]

Here's my take on it, but it's probably not right.

I'd use the back of the board for all three voltages, or I'd use a 0 ohm resistor to jump across a trace with +15v instead of going all around the chip.

If you use the back of the board I'd probably do 3 copper fills and simply use a couple vias to get the voltage as close to the capacitors as possible.

+15v +15v +15v  +15v

  gnd   gnd   IC    +15v

  gnd  gnd  gnd   +15

-15v  -15v -15v   gnd