I have been working on a 2 watt amplifier that has a Si4705 FM Tuner on the board. The amplifier that I have gone with is the PT2335 with built in tone control so you would not need to use a PT2314 or another chip. This is my first time designing for a amplifier and I hope it is decent. I would appreciate any feedback or even telling me to redo the whole thing.
My goals for the design were to have a completely free ground plane on the backside and I tried to achieve that. There is a small bridge in the ground plane between the Si4703 and PT2335. I have very little traces on the backside and I tried not to block the ground path for the amplifier when I did use the back.
This idea I like very much. I am not able to assess the correctness of the design nor wiring, but in the future I would like to build a FM receiver with digital tuning control and a digital volume control, and this could be a good basis.
Sorry, totally missed that attachment. Think I just glazed over that thinking it was the link for the top picture.
Don't know anything about the chips you are using - is the design your own, a reference design from datasheets, some combination?
This is my own design and I just took the schematic from the datasheet and I have attached the datasheet.
I wanted to be able to just plug in an arduino to it and it has the logic level converters for 5V to 3.3V for the Si4705 and then the PT2335 runs off 5V so it should be plug and play with a library.
You connect to Arduino via P6, P7?
What's the antenna going to be? Maybe review that connector, put on some kind of 75 ohm coax screw terminal.
This kind of thing, altho not this pricey of one.
The connector is a bournier and I was looking at doing a panel connector right next to it so the wires would not be long. That was the idea, would the othe connector work better?
Not sure - antenna connected right to the board would probably offer best performance tho.
Or coax cable from board to panel mount connector so that antenna impedance is maintained.
Here is with the BNC antenna connection. Added the RST connection and filled in a ground zone on the top layer along with mounting holes. Already fixed the missed connection on the level shifter. This will fit on a 5cmx10cm PCB and I'll send it off to get made shortly to see how it sounds.
The BNC mounting pegs should be grounded, not connected to RF out
K1 should have a ground pin as well. I'd use 100mil headers (PIN_ARRAY_4x1) for that connector as it's easier to get a cable for that
There are traces and vias too close to the mounting holes; the screw could short to them. Don't trust the solder mask under hardware
Traces should connect to pads or other traces at 90 degrees; acute angles can cause acid traps
I would try to route SDA/SCL away from the RF section
The +5V trace feeding the radio seems rather thin. Wider traces are better for lower impedance and less bounce
I would try to minimize cuts to the backside pour. As for the top pours, if you think they are needed, they should probably have more vias to tie them to the backside pour
You only have one via connecting the radio to ground; you may want some more. Likewize, try to visualize the ground return currents. The crystal caps, for example, have a very convoluted path back to the radio
No need to tie pins 2 and 4 on the 1117; they are one piece of metal internally. If the radio would draw more current, I would use a topside pour on those to pins to help as a heatsink, but it's not needed in this case
Make sure U3 is not installed if the reg bypass header is in the right two pins.
I would add a label to P7 identifying the voltage and polarity
P2 should have a ground; I would also label the three pins as L in, GND, R in
The traces providing 5V to the output (both sides of L2, to C8, and to the amp are too thin
All of the components above the amp chop have their ground path badly chopped by the I2C lines
