To ground pour or not? - Page 1
Forum section: electronics / projects

author: vini_i
author_rank: Regular Contributor
timestamp: January 18, 2017, 02:22:02 am
content: I designed an audio mixer board. The board mixes two microphones I'm torn on what I should do with the ground pour.Leave the ground as they are (no pour). The grounding scheme is not the best but not too bad.Flood the board on both sides. This may create inadvertent ground loops.Flood the board with a plane that is other than ground and then jumper it to ground with a zero ohm resistor or solder jumper. This would create a ground plane that does not mingle with actual ground avoiding ground loops. (i've never actually tried this)Any thoughts?

author: richard.cs
author_rank: Super Contributor
timestamp: January 18, 2017, 11:11:00 am
content: My default is to flood both sides with GND and then thoroughly stitch the two together with vias so there are no floating or weakly connected areas. It's not as good as a solid ground plane, but it's the best you can do on a 2-layer board with double-sided assembly.Generally trying to do anything else other than connect everything with a low impedance plane is risky, ground plane cuts and star grounding need careful thought if they are not to end up causing more problems than they solve.

author: dmills
author_rank: Super Contributor
timestamp: January 18, 2017, 11:49:12 am
content: Ground plane with plenty of stitching is my default position, and actually generally does just fine for audio.Star grounds in small signal audio are something you only see in amateur hour and audiophool kit, the pro stuff very seldom bothers.I would note that you are very short on bulk decoupling, a flat battery can be quite a high resistance and those little SMT ceramics are not going to cut it, I would be looking at adding a couple of 220uF electrolytics to decouple the power input and the 1/2 supply rail. I might also be looking to form an RC filter in the mic 'plug in' power line to help to keep regulator noise out of the mic inputs, a few hundred ohms and another electrolytic feels right.73 Dan.

author: steaky1212
author_rank: Regular Contributor
timestamp: January 18, 2017, 12:20:37 pm
content: Just looking at your board. I'm sure there is a good reason, but why have you got R13 and R14 in series? They look like they are just the current limiting resistors for the LED, but I don't understand why you've got 2.

author: vini_i
author_rank: Regular Contributor
timestamp: January 18, 2017, 01:00:23 pm
content: Quote from: steaky1212 on January 18, 2017, 12:20:37 pmThat was just to keep the BOM count down. I had the room and figured that adding yet another resistance value would not be beneficial. Theoretically it should be a 5k8 (if using a single resistor). I already had 2k2 value in the BOM so i put 2 in series. I also have 10k in the BOM and i may change those resistors to two 10k in parallel.

author: steaky1212
author_rank: Regular Contributor
timestamp: January 18, 2017, 01:11:32 pm
content: Quote from: vini_i on January 18, 2017, 01:00:23 pmIt's a interesting balance that relies on the method of manufacture I guess. I try to reduce the BOM lines so that it is a single run through the pick and place. In that case you pay for an extra unneeded component to save on running the board through twice. But if you already have to go through twice (or are simple enough to go through once) then I'd stick with the single resistor. Again, if I were paying someone to hand populate then I'd go with the 5k8. How bright is the LED with just a 10k resistor, obviously you cut the current in half (roughly) but it might be bright enough still.

author: BrianHG
author_rank: Super Contributor
timestamp: January 18, 2017, 09:37:30 pm
content: Ground the chassis of VR1 and VR2. It should help prevent potential external interference coming in through the metal & when adjusting the pots if the knob is also metal.Filling a ground plane on the top only (red layer) in this small design with audio bandwidth shouldn't create a problem and may be beneficial, otherwise, make you ground traces really thick if you want a partial solution inbetween the ground fill and what you have now.Also, if you are not ground filling, cut your current ground between J1 and J2, and reconnect J2's GND to VR2's GND.Also tie you power coupling capacitor after the power switch, not before.Also, if you are not Ground filling, cut the GND trace going above the power switch and instead go between the VR1 and VR2 to the GND of you OP-AMP and output connector.

author: vini_i
author_rank: Regular Contributor
timestamp: January 19, 2017, 12:55:01 am
content: I redid the design. I added a 220uF aluminum capacitor across the battery. I flooded both sides with ground and via stitched it together. Grounded the VR cases.