Please look at my first PCB

[mbar]

Hi all!
Could someone take a look at my very first PCB project and tell me if there are any major errors? This PCB is for active LR crossover, part of my active loudspeakers.

I tried to do one-sided PCB using SM devices, but it was too cumbersome for me, so few tracks are on the "second" side. Some components are TTH.
Red is top, green is bottom side. I'm a little bit afraid of the following issues:
- routing signal lines under power tracks (underneath TL074)
- GND (power) and GNDA (audio) are NOT connected on this PCB (they are connected in power supply on another PCB)
- GND and GND are planes on opposite sides -- will they crosstalk via internal capacitance?

[janneman]

Well, it's pretty hard to judge it without a schematic.
I do see a lot of wasted area.

jan diddden

[mbar]

Here you go:
http://technoportal.pl/photo/kolumny/pcb4.png

[Krisfr]

Two suggestions...

Build the circuit with Thru the hole components to make sure it works First...

Group each op amps parts and layout just those parts together, THEN combine all circuits to fit on the board...in other words build in sections.

Good luck and remember in PCB layout, symmetry is everything.

[mbar]

I already have working PCB (universal) with TTH components
Prototype is OK, but very susceptible to GSM interference.

[mbar]

Originally Posted by Krisfr

Group each op amps parts and layout just those parts together, THEN combine all circuits to fit on the board...in other words build in sections.

Good luck and remember in PCB layout, symmetry is everything.

Thanks, then I think some PCB tweaking is in order

This crossover is the last part that is keeping me from finishing my first DIY loudspeakers:


Speakers used:

Seas 27TFFC THE ART OF SOUND PERFECTION BY SEAS - H0881-06 27TFFC

STX GDN-14-100-8-SK GDN-14-100-8-SK - Niskotonowe - G?o?niki domowe - profesjonalne i tanie g?o?niki domowe - STX

[marce]

In PCB design, placement is everything, get that right and the rest will follow.
The GSM interference is prbably due to long loops created by the grounds joining back at the power supply, this is not good practice for RF interference.

[gfiandy]

Hi,

If GSM interference is a significant concern use this mind experiment to consider your approach.

Look at each node on the circuit diagram imagine attaching a signal generator with a 1GHz signal at low level and consider the passive impedance to ground. i.e the impedance without going through any silicon.

If you find nodes with a combination of high impedance and a path into your silicon then you will most likely get GSM noise.

For example the L.F filter may be OK as it has capacitors to ground in several places. At 1GHz; so long as the track lengths are short, these will direct any GSM signal to ground. If you have long track lengths then at 1GHz the inductance will prevent the capacitance from being effective. You don't need much track length, a few mm will start being a problem, so best approach is to consider it like the H.F circuit below.

The H.F filter is likely to be a problem as you have several nodes which are high impedance at 1GHz and feed straight into the input of the opamp. The opamp will be too slow to pass this signal through so it tends to rectify it causing audible noise. You could try a couple of approaches here depending on how important the immunity to GSM is.

Lowest risk is keep these paths as sort as possible and ensure that the ground plane is as close as possible. The short path length will reduce pick up, having the ground plane close will create a parasitic capacitance from the signal to ground which at 1GHz should help to redirect the signal to ground.

You can reduce the amount of signal that gets into the opamp by using series ferrite parts which will be low impedance at audio frequencies but high impedance at 1GHz. If you use this approach they should be as close to the input pins as possible.

Another possible approach is to use very small high frequency capacitors to redirect the signal away from the input. These would be a few pF and should be placed from the input pins to ground. The problem with this is they can cause instability as they appear in the pole zero response of the amplifier. If you are going to use TL074 TL072 you will probably get away with this as they are quite slow amplifiers so the capacitance effects should occur outside the 0dB gain crossing point.

Personally I would go with the shortest track lengths and closest ground plane as possible and put up with a bit of GSM breakthrough. Use vias to connect regions of the PCB that don't flood with ground plane. It is best to think of the signal flowing across the plane and allow input and output vias so current can flow in the ground.

Hope this helps,
Regards,
Andrew

[gfiandy]

At audio frequencies the grounds will not crosstalk.

At H.F the capacitance between the ground planes will make them behave as if connected. This is good for GSM rejection. You may even need to add a few pF to increase this coupling.

Signal crossing power under TL074 is OK. Try to keep crossings perpendicular this reduces any coupling.

Regards,
Andrew

[mbar]

Originally Posted by gfiandy

... consider the passive impedance to ground. i.e the impedance without going through any silicon.

If you find nodes with a combination of high impedance and a path into your silicon then you will most likely get GSM noise.

For example the L.F filter may be OK as it has capacitors to ground in several places. At 1GHz; so long as the track lengths are short, these will direct any GSM signal to ground. ...
Hope this helps,
Regards,
Andrew

Thanks, I've always known "high impedance = bad and causes HF interference" but I couldn't put my finger on "where is this high impedance in my circuit".

Thanks for all information