Creating controller for LED display, help / review needed

[muktupavels]

I have updated both boards. In both boards I tried to use polygon for power, is that good or in this case traces was better? In USB to RS485 both shields are now connected to GND. How boards looks now?

[Lt_Flash]

Now they look very nice to me! Good job putting these VCC polygons in and forming a good GND planes! You can extend VCC plane just a bit so it would connect directly to IC1 output and covering C15. Same with all component connections - you can just extend your VCC poly to cover all the contacts of resistors and capacitors, like R3,R5 and C5 can be covered by extended VCC poly instead of connecting them with a trace. And, as I said before, it would be even better if you'd use straight join instead of 3-point one.

[muktupavels]

And, as I said before, it would be even better if you'd use straight join instead of 3-point one.

You mean thermals? From what I understand they are used to make soldering easier. If that really helps then I would prefer to keep them. I don't have good temperature controlled soldering iron.

[Lt_Flash]

And, as I said before, it would be even better if you'd use straight join instead of 3-point one.

You mean thermals? From what I understand they are used to make soldering easier. If that really helps then I would prefer to keep them. I don't have good temperature controlled soldering iron.

I'm talking about polygon connect style. You're using 'Relief connect' and yes, that helps with soldering, but you really don't need any good temperature controlled iron to solder even direct connect. I'm not using my reflow gun when soldering any types of components except for BGA or QFN ones, I'm using just a soldering iron. Usually you just put some flux on one contact of resistor/capacitor/other component, solder it, using twizzers to align component, and when you're happy with alignment - just remove iron from component while holding it with twizzers, let it cool down so it holds, and then just solder another contact pad of component. And I never had any issues using direct connect polygons and soldering components with just a simple cheap soldering iron. Yes, that would take a bit more time to heat up because of polygon plane, but nothing bad would happen. But again - that's up to you, I've seen many designs where relief connect is used, as an example - Atmel's evaluation boards, like ATSAM Xplained series and others.

Here's a link to connect styles in CircuitMaker:
https://documentation.circuitmaker.com/display/CMAK/PCB_Dlg-PolygonConnectStyleRule_Frame((Polygon+Connect+Style))_CM

[Lt_Flash]

 Here's how a board with direct poly connects looks like. Also note the full GND plating on top, how C5 and L1 are connected together with a polygon and a couple of polygons for VCC and other voltages on the right.

[muktupavels]

Thanks! I decided to keep things as is for now. I am using EAGLE and it seems that your mentioned "Relief connect" is same thing as "Thermals" in EAGLE.

[Lt_Flash]

No worries at all!

[Eka]

First, a decoupling capacitor isn't needed on the DS3231 Vbat supply unless it is the only power source, Ie Vcc not connected. If it is just used for battery backup then there is no need for it. In fact having a decoupling capacitor there will drain the lithium backup battery faster.

I was looking at that long +5VDC trace. If you swapped the battery and clock with the logic level converter and atmel, and rotated the logic level converter 90 degrees, the length of the +5VDC trace would be roughly halved. Also the heavy 3.3VDC user, Atmel, would be closer to the power supply.. The clock chip uses so little power it just needs a bypass capacitor for it to be happy with it's power supply trace. I routinely power them using 5+ inch long 30 AWG VCC and GND wires with no reliability issues. The I2C carrying traces going to the Atmel can be long if needed. Just keep them the same length. On the other hand the +5VDC trace powering the logic level converter gets a workout when the LEDs are being updated.

If you need the time to be maintained for more than a couple days, feel free to ignore this. Another change I would make is swapping in a 0.47 Farad super capacitor in place of the lithium battery. A 3.3V or higher voltage super capacitor can be charged from the 3.3VDC supply using a diode, and resistor in series. The diode should have a very low forward voltage drop, and low reverse leakage current. Diodes with a reverse leakage current of 10 micro amps or less do very nicely. Search first for low forward voltage drop, then sort on increasing leakage current. Leakage currents down into the pico amps are available, but they often have relatively high forward voltage drops and cost much more. Size the resistor to set the maximum initial charge rate when the super capacitor is at 0 Volts with no charge. I use 25 to 50 mA. The charge rate will slowly lower as the super capacitor's voltage increases. It will charge up to 3.3V minus the diode forward voltage drop for < 1 mA current over a few hours. I've been using a diode that only has 0.3V drop at very low mA currents. A 2.95 Volt charge in a 0.47 Farad super capacitor will backup power the DS3231 for 2 to 4 days before it drops below the minimum voltage new temperature correction adjustments will still be calculated. My tests show the oscillator will keep working down to just under 1 Volt which takes a few more days to reach. It just looses adjustments to the temperature adjustments. 2 days should weather most power outages. Yeah, it's not years like a lithium battery, but it can be shipped with no lithium battery restrictions.

The super capacitor I've been using for my clock backup circuits is also able to be reflow soldered. No hand soldering or installing a lithium battery later. The main downside is cost. At $5.60/Q1, $3.32/Q200, the super capacitor is much more expensive than a coin cell lithium battery.

This diode CFSH05-20L from Central Semiconductor Corp is better suited than the one I use. Only 0.16V forward voltage drop at sub 1 mA currents. I may switch to it or another one.
https://www.centralsemi.com/get_document.php?cmp=1&mergetype=pd&mergepath=pd&pdf_id=CFSH05-20L.PDF

[muktupavels]

May I ask for some review, again?

Some changes:
- ATXMEGA256A3U replaced with ATSAMD51J20A.
- Removed decoupling capacitor from DS3231 vbat.
- Added crystals.
- Added DS2482S.
- Added M95256.

[Lt_Flash]

Pullup on SWCK is usually 1k as per SAMD21 or SAML21, make sure 10k is the correct one.

[muktupavels]

Thanks! Data-sheet also says 1k.

[Lt_Flash]

No worries, otherwise looks much better and professional! But I didn't check it thoroughly as I'm currently not at home Maybe just cover 3V3 output of the regulator with polygon? Till the middle of capacitor, as that's your primary 3V3 joint.

[Lt_Flash]

Also it may be a good idea to add a lot of thermal vias around and under voltage regulator for better thermal performance.

[Lt_Flash]

Just one more thing, I can see you've got a 5V trace running from connector, why don't you flip C7 upside down and then create a solid polygon for 5V rail? Just a thought, though. In regards to 3V3 rail - you often have different cover of the polygon over capacitor contacts, like at C1 or C5 - it's just a tiny 10mil trace, actually, even though you have a whole huge polygon next to it. Just cover the half of capacitor with that polygon everywhere, right to the middle of each cap, not the way you have it - different for each capacitor, that'd be good. Otherwise - seems good to me. Polygons can be optimized a bit, but nothing to be stressed about.

[Lt_Flash]

Here's a good video from Dave about bypass caps and where to place them, just for information.

[Eka]

Just a thought, though. In regards to 3V3 rail - you often have different cover of the polygon over capacitor contacts, like at C1 or C5 - it's just a tiny 10mil trace, actually, even though you have a whole huge polygon next to it. Just cover the half of capacitor with that polygon everywhere, right to the middle of each cap, not the way you have it - different for each capacitor, that'd be good. Otherwise - seems good to me. Polygons can be optimized a bit, but nothing to be stressed about.

The short traces between solder pad and flood fill polygon* is done is for easier soldering, and if mass produced it would be much less likely to have gravestones. Electrically it means very little because the traces are so short.

* I forget what they are called.

[Lt_Flash]

Just a thought, though. In regards to 3V3 rail - you often have different cover of the polygon over capacitor contacts, like at C1 or C5 - it's just a tiny 10mil trace, actually, even though you have a whole huge polygon next to it. Just cover the half of capacitor with that polygon everywhere, right to the middle of each cap, not the way you have it - different for each capacitor, that'd be good. Otherwise - seems good to me. Polygons can be optimized a bit, but nothing to be stressed about.

The short traces between solder pad and flood fill polygon* is done is for easier soldering, and if mass produced it would be much less likely to have gravestones. Electrically it means very little because the traces are so short.

* I forget what they are called.

Yes, I know what relief connect is for, but usually you would want to pour polygon around pad so there would be three short traces to polygon from a pad. It may be important for power rails.

[muktupavels]

Maybe just cover 3V3 output of the regulator with polygon? Till the middle of capacitor, as that's your primary 3V3 joint.

Did I understand this correctly? Please check new attachment...

Also it may be a good idea to add a lot of thermal vias around and under voltage regulator for better thermal performance.

Added only under regulator, is that ok?

Just one more thing, I can see you've got a 5V trace running from connector, why don't you flip C7 upside down and then create a solid polygon for 5V rail? Just a thought, though.

Is not trace big enough?

In regards to 3V3 rail - you often have different cover of the polygon over capacitor contacts, like at C1 or C5 - it's just a tiny 10mil trace, actually, even though you have a whole huge polygon next to it. Just cover the half of capacitor with that polygon everywhere, right to the middle of each cap, not the way you have it - different for each capacitor, that'd be good.

Done. Is that what you meant?

Here's a good video from Dave about bypass caps and where to place them, just for information.

Thanks, but I have seen that video. The real question is whether I have learnt something from it...  Probably should watch again.

In few places I have put vias to connect top gnd polygons that are split by 3v3. Is that needed?

[Lt_Flash]

Yes, you did understand correctly, now you have a solid 3-wire connections for each 3V3 rail! Thermal vias are good too, there's a solid polygon around that regulator and now with thermal vias even if regulator would get hot - these vias will help to dissipate heat. In regards to 5V rail - yes, trace is usually enough, I just got used to use polygons where possible with power rails, usually that's better, it also dissipates heat and has better conductivity too. In regards to GND vias - usually you would want to have them as that shortens your current return path, thus reducing impedance of a trace.

[Lt_Flash]

Just one more thing - you probably would want to cover pin 3 of regulator with 3V3 polygon, that's why I included Dave's video, it says that you should have decoupling capacitor as close to regulator output as possible even if that's a polygon pour, but in your case it's just a short thick trace and then a huge polygon, so current would flow through that trace first. It's better to have a polygon and a cap close to the source of current, as I suggest.

[Lt_Flash]

Sorry, my mistake, you're doing a thermal relief connection style for polygons, in that case - no need to cover pads with polygon as it will produce three thinner connections instead of your beefy one! I just so got used to have direct connect style that I'm making such stupid mistakes

[Lt_Flash]

And another though - because you've got such a big 3V3 polygon and just a single connection from regulator - you may want to put some beefy tantalum cap somewhere on 3V3 rail, something like 47uF or 22uF or at least 10uF - that would help to keep 3V3 steady in case when fast switches of levels are generated by MCU, for example and would smooth output ripple of regulator. I'm not sure how much current would your board draw but usually it's a good idea to have such cap on 3V3 or any other power rail along with bypass cap (100nF - 1uF).

[Lt_Flash]

Final thought, I'm not sure if you have checked this document yet, but here's a full design documentation for SAMD51/E54 Xplained Pro board, I'd choose same decoupling caps on all the pins of the MCU to guarantee it's stable performance. I'm not saying your design is incorrect, but maybe you just want to check it against a real production board that uses such MCU. That's what I usually do in my designs. Hope this helps!

http://ww1.microchip.com/downloads/en/DeviceDoc/SAM_E54_Xplained_Pro_Design_Documentation.zip

[Lt_Flash]

Just out of curiosity - why did you choose such a powerful and complex MCU? Do you really need it? Because there are models like SAMD21, SAML21 in a 32-pin package and with 48MHz and full-speed USB onboard, or even in a SOIC-14 package, if you don't need to many GPIO ports. Easier to do a PCB for these ones, easier to debug and with almost all features. FPU is great and 120MHz too, but as far as I understand - you just need to talk to RS485 bus and to display, I2C and SPI buses? All that can be achieved with SAMD2x/L2x MCUs without any trouble. Also, external crystals are only required if you really want a high-precision stability, from my experience I had no issues to use internal oscillators of these MCUs, didn't notice any significant (to my applications, including FreeRTOS) time drift, but they allow to save a lot of power if you're operating from a battery or switched into a battery backup mode. SAML-series MCUs are the best for lowest power applications. In regards to external crystals - you also want traces to them to be as short as possible and of equal length for best stability.

[muktupavels]

In regards to GND vias - usually you would want to have them as that shortens your current return path, thus reducing impedance of a trace.

Thanks!

And another though - because you've got such a big 3V3 polygon and just a single connection from regulator - you may want to put some beefy tantalum cap somewhere on 3V3 rail, something like 47uF or 22uF or at least 10uF - that would help to keep 3V3 steady in case when fast switches of levels are generated by MCU, for example and would smooth output ripple of regulator. I'm not sure how much current would your board draw but usually it's a good idea to have such cap on 3V3 or any other power rail along with bypass cap (100nF - 1uF).

I think I only have two electrolytic caps - 10uf and 100uf:
- https://www.digikey.lv/product-detail/en/panasonic-electronic-components/EEA-GA1C100B/P15786CT-ND/3831153
- https://www.digikey.lv/product-detail/en/panasonic-electronic-components/EEA-GA1C101B/P15796CT-ND/3831163

Will 100uf be good enough or I really need tantalum?

Final thought, I'm not sure if you have checked this document yet, but here's a full design documentation for SAMD51/E54 Xplained Pro board, I'd choose same decoupling caps on all the pins of the MCU to guarantee it's stable performance. I'm not saying your design is incorrect, but maybe you just want to check it against a real production board that uses such MCU. That's what I usually do in my designs. Hope this helps!

http://ww1.microchip.com/downloads/en/DeviceDoc/SAM_E54_Xplained_Pro_Design_Documentation.zip

All pins? I think I have decoupling cap on every power pin, did I miss something?

I have seen that and I have pdf open still... That board use 128 pin device, but I have 64 pin...

Just out of curiosity - why did you choose such a powerful and complex MCU? Do you really need it? Because there are models like SAMD21, SAML21 in a 32-pin package and with 48MHz and full-speed USB onboard, or even in a SOIC-14 package, if you don't need to many GPIO ports. Easier to do a PCB for these ones, easier to debug and with almost all features. FPU is great and 120MHz too, but as far as I understand - you just need to talk to RS485 bus and to display, I2C and SPI buses? All that can be achieved with SAMD2x/L2x MCUs without any trouble. Also, external crystals are only required if you really want a high-precision stability, from my experience I had no issues to use internal oscillators of these MCUs, didn't notice any significant (to my applications, including FreeRTOS) time drift, but they allow to save a lot of power if you're operating from a battery or switched into a battery backup mode. SAML-series MCUs are the best for lowest power applications. In regards to external crystals - you also want traces to them to be as short as possible and of equal length for best stability.

32 MHz xmega was not fast enough. Text was scrolling too "slow", I was hoping that I could workaround that by moving content by multiple positions at one time, but that had side-effect - text suddenly looks very bold...

I don't want to redo pcb if internal oscillator will not be good enough. That pcb will be outside of building and has to work in winter and/or summer and from what I have read temperature can affect stability.