Lab Power Supply - Board Redesign

So in the last post I was at the point where I felt I had ironed all the faults out of the current design and felt it was time to go for a new board. Since then I rolled all the changes back into the schematics and designed a new board that integrates all those changes.

Schematic Changes

So I will go through each section of the schematic, list the changes and then include the updated schematic.

Power

In this section I made the following changes:

1. I added a diode across the relay to suppress back-EMF when the relay is switched-off.
2. I changed the 24V LM317 to be a TO-220 package as the surface-mount version was getting too hot.

Pre-Regulator

In this section I made the following changes:

1. A buffer for the Ioutmon (U14) and Voutmon (U7D) signals to stop them affecting each other through the summing amplifier. This was causing the voltage to vary under load and causing incorrect current readings at low currents.
2. A peak-detector (D12, C28, R52) to slow down the decrease in the pre-regulator when the voltage drops. This helps stabilize the output when a pulsed load is driving the system into current limit
3. A minimum voltage of 0.6 + 3.3V to the pre-regulator (D13, D15, D14, R57). This prevents the pre-regulator going down to zero when the output voltage is very low (for example if you set the current limit to a very low value like 20mA)
4. A bypass capacitor for U7 (was missing from previous schematic).

Post Regulator

In this section I made the following changes:

1. The orientation of Q8 was corrected (collector and emitter where the wrong way round due to a footprint change when I changed the component model).
2. The differential amplifier measuring the output voltage was changed to use 100K resistors and the compensation capacitor was reduced to 4.7pF. This increases the impedance of the amplifier inputs but then the compensation had to be reduced to maintain the same response time.
3. I removed the four terminal voltage sensing. This wasn't stable and I didn't want to mess around to fix it so for now I am not supporting sense terminals. I will still sense the voltage at the output terminals but you can't connect sense wires to an external load.
4. The MOV output protection was changed to just 2 MOVs. This is as a result of the change to only have two terminals instead of 4.
5. The current sense resistor was changed to the Vishay VC1625. While the tempco and accuracy of the Welwyn OAR3 resistor was fine, the thermoelectric effect wasn't. I decided to go with a higher precision four terminal current sense resistor.

PCB Changes

I have been struggling to find a case that will house the project and then the recent discovery that I needed to put the bridge rectifier on the heatsink led me to re-think the problem. In addition to the bridge I need to include another TO-220 for the 24V supply which means I need to make the board much wider.

The heatsink I chose is 254mm wide (10") so there is no option to put three modules on one heatsink. I figured out that if I can reduce the length of the board to below 100mm the project will fit comfortably fit inside a 3U 19" rackmount case. 3U gives me 130mm of height for the Raspberry Pi touch screen which leaves around 30mm of height for binding posts.

The 19" case however is 480mm wide which gives me lots of space. I realized that if I got another heatsink and cut it in half (so 125mm wide) I could fit this in the case also and still get three channels.

Layout Changes

Having the bridge on the back edge makes some things a bit tricky. The bridge needs to be near the relay, the pre-regulator MOSFETs, the capacitors. The VCC bridge also needs to be nearby also but this creates a problem if the power connector is at the edge of the board as some traces would need to be router right over the other side to get to the internal voltage regulators.

Instead I put the internal regulators (for VCC, 5V, 24V) on the left side, the power connector, relay and bridge in the middle and then the pre-regulator MOSFETs and output MOSFET toward the right.

The pre-regulator circuit (except for the opamps) is at the top right near the pre-regulator MOSFETs. The bulk capacitors are between this and the output.

The analog section is at the front near the middle and then the digital section is to the left (section with ground plane). The USB section is below the internal regulators and behind the other digital sections. It wasn't practical to put the USB connector at the edge of the board so this too is in the middle nearer to the power input.

I also used 4mm traces for the heavy current tracks which allowed me to make the board quite compact. 

This worked quite well overall as none of the power traces are very long, the analog bits of the digital section are close to the analog section and the analog section is close to the negative output (which is the ground point for the circuit) and the sense resistor.

The layout is much more dense than before so there are a few more vias. The control lines for the relay transistor, the VCC voltage control and the signal that controls the pass transistor were particularly difficult to route.

I was able to fit nearly everything in with 80mm of width but I couldn't figure out how to rout the Vrelay and Vsetplus lines. I ended up adding an extra few mm of width so the board is 128mm instead of 125mm. This will have a negligible effect except that there will be a slight overhang off the ends of the heatsink.

Here is how the board looks in 3D - not all parts have models.

Other layout corrections:

1. The ground routing for the analog and digital section all comes off one track that connects right at the sense resistor. Before some of the grounding came off an earlier point on the heavy-current ground path and this created some voltage differences.
2. The PTC was placed further from the sense resistor to avoid temperature induced errors.
3. The placement of the capacitors for the AD7705 crystal were too close so these were placed a bit further off.
4. A bit more space was added between the pass transistor and the pre-regulator MOSFETs to allow the aluminium dioxide insulator pad to fit.

Footprint Changes

1. The MOV footprint was mirrored before (made sense from bottom of board). This was corrected.
2. The PTC footprint was mirrored before. This was corrected. Also the footprinted suggested by the manufacturer had the feet too far off the axis of the part so I reduced this a bit to make the part fit more comfortably.
3. The MCP2200 footprint was the wrong width and this was corrected
4. The AD7705 was changed to be the SOIC footprint as I got some of these cheaply off ebay.
5. The pads for the main capacitors were too small. I added bigger pads for better mechanical strength.
6. The LM317 used for 24V rail got too hot as a surface mount component so this was changed to a TO-220 part.

Next

So I have ordered more boards from Seeed studio and am waiting for these to be manufactured. Next step will be assembling and testing the channel on the new board.