Hi. I'm finally ready (took me 4 years!) to build my proper 2.1 chip amp. This is the layout i came up with, I was wondering if it's OK (don't worry about component sizing as I need to find what's locally available and work from that).
I tried to make a star ground (I use Eagle's POLYGON and lines in the bRestrict layer, this effectively "cuts" the polygon in the places i want, making a star ground and carefully cutting off all loops).
I tried to make a star ground (I use Eagle's POLYGON and lines in the bRestrict layer, this effectively "cuts" the polygon in the places i want, making a star ground and carefully cutting off all loops).
First make a list of design goals, star ground can be one.
How do you want to place the bypass capacitors or route the input? Should you closely route supplies and returns? Where do you need low inductance routing? What is the best power supply configuration? If its a multi channel amp how will you connect the amps to the power supply? Ground loops? Feedback loop? ..........................
How do you want to place the bypass capacitors or route the input? Should you closely route supplies and returns? Where do you need low inductance routing? What is the best power supply configuration? If its a multi channel amp how will you connect the amps to the power supply? Ground loops? Feedback loop? ..........................
Why limit yourself to one layer? You'll get better performance with a ground plane on one side of the board, supply pours on the other. See example here: http://www.diyaudio.com/forums/chip-amps/252436-lm3886-pcb-vs-point-point-data-21.html#post3899248
~Tom
~Tom
Double sided, supply rails as far from signal rails, supply rails +- as close together as possible. HF filters as close to supply pins as possible, keep your supply rails wide and similar to eachother as possible. Round curves are always better than sharp 90° corners.
On both signal and supply side. Ground planeitsquite good idea...
No speaker GND on PCB. Id rather use .125 or .250mW resistors because theres no need for high wattage ones. Im not an expert on this anyway.... 🙂
On both signal and supply side. Ground planeitsquite good idea...
No speaker GND on PCB. Id rather use .125 or .250mW resistors because theres no need for high wattage ones. Im not an expert on this anyway.... 🙂
I have to use single-layer because it's what i can make at home. This is a weekend project (I'm looking to finish it this weekend). I can't have boards made, or buy online, since I'm in Argentina and it takes 2-3 MONTHS to deliver here (customs delays). I can make double-sided at home but I don't have the ability to make vias, and alignment is always hard to get 100% right so I prefer to avoid it.
I like the idea of no speaker GND on PCB, didn't think if that.
This is a multi-channel amp (stereo + sub), so I'll have a power supply with big capacitors, and then point-to-point power distribution to each amp.
Bypass caps are C1/C2 (big ones) and C4/C5 (ceramics). I placed them as close as possible to the supply pins of the IC.
The only issue i can think of is input signal ground: since each amp is independent, connecting a stereo output will effectively make a loop in the signal ground cable. I think this could be solved by "ground lift" (connect the shielding of the cable to ground in one end only).
I like the idea of no speaker GND on PCB, didn't think if that.
This is a multi-channel amp (stereo + sub), so I'll have a power supply with big capacitors, and then point-to-point power distribution to each amp.
Bypass caps are C1/C2 (big ones) and C4/C5 (ceramics). I placed them as close as possible to the supply pins of the IC.
The only issue i can think of is input signal ground: since each amp is independent, connecting a stereo output will effectively make a loop in the signal ground cable. I think this could be solved by "ground lift" (connect the shielding of the cable to ground in one end only).
I make double-sided PCBs in my garage using the toner transfer method. As you mention the alignment is tricky. I cut the printout of the board layout leaving a 1 cm margin. Then I tape the top and bottom layouts to a piece of scrap PCB material. If you place them on a light table (or hold them up against a window in daylight) you can align top and bottom layers to within +/-0.2 mm without too much trouble. I preheat the board and sandwich it between the top and bottom layout printout feeding everything through the laminator at once.
Vias can be made by soldering a piece of wire in a hole. Generally, I try to make connections between top and bottom layers at the component pins rather than using vias. You don't need thru-plated holes. Just solder on top and bottom sides.
~Tom
Vias can be made by soldering a piece of wire in a hole. Generally, I try to make connections between top and bottom layers at the component pins rather than using vias. You don't need thru-plated holes. Just solder on top and bottom sides.
~Tom
i can say that your PCB layout is not good...
too many angles, unnecessary one... current do like 90 degree connections.
too many angles, unnecessary one... current do like 90 degree connections.
Here's an updated version of the board. Highlighted is the ground pour, as you can see there is no star ground in this version, but I tried to keep all "high power" ground separated from signal ground. The ground planes are split but they connect right at the left of R2.
I made a version of this board last night and I'll be testing it today.
I made a version of this board last night and I'll be testing it today.
I fell foul of smoothing capacitors charging current impulses modulating the audio ground.
The power supply needs to come in first to the smoothing capacitors then out the other side to the amplifier.
Decoupling should be close to IC or it might oscillate.
+1 for speaker ground connected at power supply mid point.
The power supply needs to come in first to the smoothing capacitors then out the other side to the amplifier.
Decoupling should be close to IC or it might oscillate.
+1 for speaker ground connected at power supply mid point.
The only thing that I would change would be to move the -ve rail so that it ran along the back of the board so there was some ground plane between the rails and rearrange C1 and C2 so that their ground connections are right next to each other on the ground between the rails and possibly rearrange C4 and C5 too, but in saying that it's probably fine as it is
A few more suggestions:
Move R1 closer to the chip.
Remove the audio ground plane. Use closely placed supply and return traces.
Connect C7 to PG instead of AG.
I like to use + GND and - GND for the PSU connections, building a four rail PSU and only connecting the grounds together at the AMP.
Move R1 closer to the chip.
Remove the audio ground plane. Use closely placed supply and return traces.
Connect C7 to PG instead of AG.
I like to use + GND and - GND for the PSU connections, building a four rail PSU and only connecting the grounds together at the AMP.
Except that the LOOP AREA of the input is far too big.
The PCB layout shows the Signal Return going all the way to a remote Star Ground and then comes all the way back again.
The first part of that excess routing has a BIG Loop Area.
The second part, has close coupled traces, which have small Loop Area.
The R connected to -IN goes to the NFB DC blocking cap, to the star ground and back to the Signal Return. That has a BIGGER LOOP AREA than the first part mentioned above.
The Signal Flow and Return should be close coupled all the way from the external Sourve equipment right up to the +IN and -IN Pins.
Then take one trace from Signal Return to the Main Audio Ground/Star ground to allow the chip to reference the input voltage to the output voltage.
The PCB layout shows the Signal Return going all the way to a remote Star Ground and then comes all the way back again.
The first part of that excess routing has a BIG Loop Area.
The second part, has close coupled traces, which have small Loop Area.
The R connected to -IN goes to the NFB DC blocking cap, to the star ground and back to the Signal Return. That has a BIGGER LOOP AREA than the first part mentioned above.
The Signal Flow and Return should be close coupled all the way from the external Sourve equipment right up to the +IN and -IN Pins.
Then take one trace from Signal Return to the Main Audio Ground/Star ground to allow the chip to reference the input voltage to the output voltage.
I should buy a boat.
Where else should that NFB cap go then? AndrewT has the view of an eagle that has some serious knowledge about electrical design.
I have that PCB in the other computer I normally dont use and its far away from where I really am so.. I cant fix those mistakes.
I see what you mentioned and know how to fix them but maybe later.
Where else should that NFB cap go then? AndrewT has the view of an eagle that has some serious knowledge about electrical design.
I have that PCB in the other computer I normally dont use and its far away from where I really am so.. I cant fix those mistakes.
I see what you mentioned and know how to fix them but maybe later.
Last edited:
keep the -IN trace really close to the +IN trace.
Both traces have a series pair of resistor+capacitor.
Place them alongside each other.
- Status
- Not open for further replies.