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?
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?
An externally hosted image should be here but it was not working when we last tested it.
An externally hosted image should be here but it was not working when we last tested it.
An externally hosted image should be here but it was not working when we last tested it.
Well, it's pretty hard to judge it without a schematic.
I do see a lot of wasted area.
jan diddden
I do see a lot of wasted area.
jan diddden
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.
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.
I already have working PCB (universal) with TTH components 🙂
Prototype is OK, but very susceptible to GSM interference.
Prototype is OK, but very susceptible to GSM interference.
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:
An externally hosted image should be here but it was not working when we last tested it.
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
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.
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.
Last edited:
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
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
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
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
Last edited:
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 🙂
OK, version 2 below, I think this is as good as it gets considering that I'm a beginner at PCB design.
An externally hosted image should be here but it was not working when we last tested it.
An externally hosted image should be here but it was not working when we last tested it.
An externally hosted image should be here but it was not working when we last tested it.
An externally hosted image should be here but it was not working when we last tested it.
An externally hosted image should be here but it was not working when we last tested it.
Hi,
This is a good design, I have made some further observations but it will work OK as it is.
I would add some mounting holes otherwise it will be a pain trying to fit it to your cabinet.
If it is going to be manufactured with a silk screen it needs tidying up otherwise there is no point paying for it.
You could shorten it significantly by putting the regs next to the caps. This will save money if you plant to have it made by a PCB company. If you are going to do it yourself the extra cost of board is probably not worth the effort.
The ground plane could be improved by shuffling some of the parts and tracks to make room for the flood to get round parts. This will improve screening to GSM. The return path from the decoupling caps on the TL074 has to go right round the outside of the PCB at the top, it might be possible to improve this with a couple of ground links on the bottom layer without breaking up the signal ground too much.
Regards,
Andrew
This is a good design, I have made some further observations but it will work OK as it is.
I would add some mounting holes otherwise it will be a pain trying to fit it to your cabinet.
If it is going to be manufactured with a silk screen it needs tidying up otherwise there is no point paying for it.
You could shorten it significantly by putting the regs next to the caps. This will save money if you plant to have it made by a PCB company. If you are going to do it yourself the extra cost of board is probably not worth the effort.
The ground plane could be improved by shuffling some of the parts and tracks to make room for the flood to get round parts. This will improve screening to GSM. The return path from the decoupling caps on the TL074 has to go right round the outside of the PCB at the top, it might be possible to improve this with a couple of ground links on the bottom layer without breaking up the signal ground too much.
Regards,
Andrew
Agreed. You could move U4 & U5 outward, slide the electrolytics inward and get a much more compact, rectangular-ish PCB. Not only cheaper but probably also better electrically.
jan didden
Thanks 🙂
Mounting holes -- I'll drill them myself during mounting, placing is not critical (plenty of free space inside cabinets 😉).
Yes, I'm going to order making PCBs in PCB company, and I think solder mask is a must.
Good you told me about GND return path for decoupling, I'll try to do some tweaking.
And yeah, U4 & U5 are going outwards.
Mounting holes -- I'll drill them myself during mounting, placing is not critical (plenty of free space inside cabinets 😉).
Yes, I'm going to order making PCBs in PCB company, and I think solder mask is a must.
Could you tell me what do you have in mind?
Good you told me about GND return path for decoupling, I'll try to do some tweaking.
And yeah, U4 & U5 are going outwards.
Hi
If you are going to have it manufactured might as well put 3.2mm holes with 4mm PADs at each corner to mount it; it will hardly cost anything extra and will save you the effort. It will also ensure the holes are electrically isolated, otherwise you run the risk of your mounting pillars shorting the top and bottom planes together.
The silk screen shows many of the reference designators in the middle of the part and some of them on the PADs. The PCB manufacturer will most likely make sure no silk screen is actually screened onto the pads but its bad practice to do this, if it does end up on the pads it make it really hard to solder.
If the reference designator is under the part it makes it hard to find the parts once they have been placed. Also sometimes the silk screen is thick enough to make mounting of SMT parts unreliable.
Regards,
Andrew
If you are going to have it manufactured might as well put 3.2mm holes with 4mm PADs at each corner to mount it; it will hardly cost anything extra and will save you the effort. It will also ensure the holes are electrically isolated, otherwise you run the risk of your mounting pillars shorting the top and bottom planes together.
The silk screen shows many of the reference designators in the middle of the part and some of them on the PADs. The PCB manufacturer will most likely make sure no silk screen is actually screened onto the pads but its bad practice to do this, if it does end up on the pads it make it really hard to solder.
If the reference designator is under the part it makes it hard to find the parts once they have been placed. Also sometimes the silk screen is thick enough to make mounting of SMT parts unreliable.
Regards,
Andrew
Nice to see loads of copper.
Only criticism is that there is loads of free space, the pcb could be shrunk down quite a bit.
You have got everything on there, you can now close it all in and make a smaller pcb.
Only criticism is that there is loads of free space, the pcb could be shrunk down quite a bit.
You have got everything on there, you can now close it all in and make a smaller pcb.
OK, will order PCB with holes and I'm going to move ref. designators out of pads area.
Also I'll try to make this PCB a little smaller in power supply area.
Looks like you are using Kicad. This is a pretty good program and if you want it to fill ground in areas it hasent yet, that can be accomplished by adjusting parameters in the Fill command. If those areas end up not being conneted to existing ground, traces may have to be moved. Generally you are moving right along with your cad effort.
Yeah, Kicad 🙂
As I'm a Linux user, there was no way using something else, and yes, Kicad now is a very powerful product. Suits all my needs, especially after installing some additional modules/libraries/3d models.
I hope to finish my PCB during the weekend.
BTW I have one concern that maybe should go into its own thread: the capacitor (100pF) that shunts the Input1 (to keep RF out of the PCB) presents a capacitative load for the previous stage. considering that the previous stage is almost for sure an output operational amplifier in an external preamp, it this really a good way to attenuate RF?
I mean that in almost any operational amplifier datasheet there is a warning against too big capacitance on output, and 100 pF is not considered "small" in this regard.
What could be better than shunt capacitance on input?
As I'm a Linux user, there was no way using something else, and yes, Kicad now is a very powerful product. Suits all my needs, especially after installing some additional modules/libraries/3d models.
I hope to finish my PCB during the weekend.
BTW I have one concern that maybe should go into its own thread: the capacitor (100pF) that shunts the Input1 (to keep RF out of the PCB) presents a capacitative load for the previous stage. considering that the previous stage is almost for sure an output operational amplifier in an external preamp, it this really a good way to attenuate RF?
I mean that in almost any operational amplifier datasheet there is a warning against too big capacitance on output, and 100 pF is not considered "small" in this regard.
What could be better than shunt capacitance on input?
Any good source component will have a series resistor in the output usually between 47R and 470R depending on the opamp. This has two functionone is to isolate the opamp from cable oan load capacitance and the other is to prevent the opamp from being damaged if it is shorted.
Regards,
Andrew
Regards,
Andrew
- Status
- Not open for further replies.