please check over my design and let me know how i went

[Jbates58]

hi all.

this is my first actual schematic and pcb design.

https://easyeda.com/jbates58/Current_Sensor-eabffc51781340eb8298b4af16f175ec

could you please check it over and let me know if i can make any improvments to it?

basicly, its a current and voltage sensor that i want to use for a solar display board for products i sell (showing that the right components actually make a big difference to the final product).

so the idea is 2 panels the same, are put through the solar + header. then the battery+ goes to the battery, and the load+ sits on the load line.

the only thing i have yet to do is to get the main power traces from the main headers along the top of the board to the sensors. i have chosen the 30A capable ACS712. but am not sure how to put in a big enough trace to the pads for the IC.

thanks.

Jason

[woody]

the only thing i have yet to do is to get the main power traces from the main headers along the top of the board to the sensors. i have chosen the 30A capable ACS712. but am not sure how to put in a big enough trace to the pads for the IC.

I ran into the same problem with Kicad. What I did to solve this is create a special footprint for the ASC712. On this footprint pin 1+2 and pin 3+4 share a larger pad. That allows you to connect fatter traces to the thing without running into all kinds of separation limits.

[Jbates58]

the only thing i have yet to do is to get the main power traces from the main headers along the top of the board to the sensors. i have chosen the 30A capable ACS712. but am not sure how to put in a big enough trace to the pads for the IC.

I ran into the same problem with Kicad. What I did to solve this is create a special footprint for the ASC712. On this footprint pin 1+2 and pin 3+4 share a larger pad. That allows you to connect fatter traces to the thing without running into all kinds of separation limits.

ahh yes, manes sense. can this be done with easyeda? i'll admit. this is the first time i have use id. so its been a good learning excercise.

thanks.

Jason

[ElektroQuark]

In KiCad you can manage this kind of connections with zones.

[hcglitte]

The sensor chips have no power connected to them.

There is not any decoupling capacitors for neither the the MCUs nor the sensor chips.

Why use two LCDs and MCUs? You can use one LCD and one MCU. If you need more analog inputs, use an analog MUX.

The XTALs are routed very far away from the MCU. The tracks should be short.

I would add a cap at the MCY reset line also for noise suppression.

[woody]

In KiCad you can manage this kind of connections with zones.

As I am moving away from Eagle Pro to KiCad and hence on a learning permit, are zones a better answer to this problem?

[ElektroQuark]

You can apply them to any pad distribution, so I think is a better approach.

[woody]

You can apply them to any pad distribution, so I think is a better approach.

Ah, like so. This is indeed easier, it saves making a footprint. Thanks for the tip! Now only to find out how to get rid of the airwires. 

(Attached the same piece of PCB as above)

[pix3l]

Hi Jason,
Not bad for a first ;-) But here are some points of advice:
-Try to put your crystals as close to the pins of the microcontroller(s) as possible, with the capacitors next to them
-I see some traces which are direct lines from for example R6 to the LCD. This is considered very unaesthetic, try to use only 45/135 degree angles.
-Why not put R6 above the LCD?
-I see you used 8 mil track width on your PCB. This is very small, a lot of PCB manufacturers will charge more for PCBs with tracks narrower than 0.15mm. I usually go for 0.2mm or 0.254mm so that any PCB fab can make it.
-Have you made a netlist? When I remove a track I don't see a line suggesting that something should be connected...
-Try using a ground plane for all your GND connections

Good luck!

Edit: oh and where do your ACS712's get their VCC? ;-)

[Jbates58]

Hi Jason,
Not bad for a first ;-) But here are some points of advice:
-Try to put your crystals as close to the pins of the microcontroller(s) as possible, with the capacitors next to them
-I see some traces which are direct lines from for example R6 to the LCD. This is considered very unaesthetic, try to use only 45/135 degree angles.
-Why not put R6 above the LCD?
-I see you used 8 mil track width on your PCB. This is very small, a lot of PCB manufacturers will charge more for PCBs with tracks narrower than 0.15mm. I usually go for 0.2mm or 0.254mm so that any PCB fab can make it.
-Have you made a netlist? When I remove a track I don't see a line suggesting that something should be connected...
-Try using a ground plane for all your GND connections

Good luck!

Edit: oh and where do your ACS712's get their VCC? ;-)

ok, thanks. i have fixed the few errors i have made, and re-designed the layout.

however, i just cant workout how to do a ground plane. and clues?

here is the new setup, with relocated parts. and thicker traces. but looking for the ground plane part.
(its the second PCB Layout)

https://easyeda.com/jbates58/Current_Sensor-eabffc51781340eb8298b4af16f175ec


Jason

[Jbates58]

Hi Jason,
Not bad for a first ;-) But here are some points of advice:
-Try to put your crystals as close to the pins of the microcontroller(s) as possible, with the capacitors next to them
-I see some traces which are direct lines from for example R6 to the LCD. This is considered very unaesthetic, try to use only 45/135 degree angles.
-Why not put R6 above the LCD?
-I see you used 8 mil track width on your PCB. This is very small, a lot of PCB manufacturers will charge more for PCBs with tracks narrower than 0.15mm. I usually go for 0.2mm or 0.254mm so that any PCB fab can make it.
-Have you made a netlist? When I remove a track I don't see a line suggesting that something should be connected...
-Try using a ground plane for all your GND connections

Good luck!

Edit: oh and where do your ACS712's get their VCC? ;-)

ok, thanks. i have fixed the few errors i have made, and re-designed the layout.

however, i just cant workout how to do a ground plane. and clues?

here is the new setup, with relocated parts. and thicker traces. but looking for the ground plane part.
(its the second PCB Layout)

https://easyeda.com/jbates58/Current_Sensor-eabffc51781340eb8298b4af16f175ec


Jason

ha. i worked out the ground plane. cool. i have made the base layer as a ground plane. is this good practice?

and another thing i have noticed, is that even though i have made the bottom layer the ground plane, i still have a heap of GND traces between components. wouldnt it be easier for it (as its all through hole) to just punch it through to the bottom layer and have the pad connected directly to it? is there some basic thing i have missed? i feel that if it does this it will remove alot of the wires on the top layer.

Jason

[pix3l]

Hi Jason,

Cool! Couple of more comments:
-GND plane on the bottom layer is fine but you are making a lot of small GND islands because the traces are separating these areas. Two things you can do: 1: try to keep the lines on the bottom layer as short as possible or 2: also put a ground plane on the top layer and connect the two planes with a lot of vias.
-Please look into decoupling of your ACS712 chips and microcontrollers (100nF should be fine)
-ACS712 is not recommended for new design, which means the manufacturer is (planning for) phasing out this chip. The recommended substitute is the ACS723
-Do you have any idea how much the supply current will be? If it will be more than  1 Ampere you might want to make the traces from your main power connector wider than 10 mil.

May the force be with you!

[Jbates58]

Hi Jason,

Cool! Couple of more comments:
-GND plane on the bottom layer is fine but you are making a lot of small GND islands because the traces are separating these areas. Two things you can do: 1: try to keep the lines on the bottom layer as short as possible or 2: also put a ground plane on the top layer and connect the two planes with a lot of vias.
-Please look into decoupling of your ACS712 chips and microcontrollers (100nF should be fine)
-ACS712 is not recommended for new design, which means the manufacturer is (planning for) phasing out this chip. The recommended substitute is the ACS723
-Do you have any idea how much the supply current will be? If it will be more than  1 Ampere you might want to make the traces from your main power connector wider than 10 mil.

May the force be with you!

i have filtering caps.

C13 (100nF) is the main power filter cap between Power + & -.
C12 (100nF) is the filter cap output from U3 (LM7805) to the arduino and 3 of the current sensors.
C7 (100nF) is the filter cap output from U4 (LM7805) to the arduino and 3 of the current sensors.

or have i got it wrong? but looking at the schematic, it looks correct to me.

i will substitute the ACS712 chips with the ACS723 40A chips.

how do i set it so that when the PCB is manufactured, they leave the copper pads from the screw terminals exposed, that way i can beef them up with some solder. as i am sure the traces are not sufficent for the 15-17A i wish to measure. however, if i can now measure above 30A with the new IC's then even better. that will allow me to test more products.

[pix3l]

Hi Jason,

Usually you want to have decoupling on every VCC pin of every component. See "Typical Application" schematic in the datasheet.

https://easyeda.com/Doc/Tutorial/FAQ.htm#How-to-add-solder-mask

[Jbates58]

Hi Jason,

Usually you want to have decoupling on every VCC pin of every component. See "Typical Application" schematic in the datasheet.

https://easyeda.com/Doc/Tutorial/FAQ.htm#How-to-add-solder-mask

ok. well thats done. and i have added a ground layer to the top layer aswell. so i think it should nearly be good to go.

and thanks heaps for the solder layer info. exactly what i was after.

so, if this is all well and good, any tips for where i should get it made? is the supplier that easy eda send it to sufficent?

Jason

[pix3l]

Good work! I have ordered PCBs multiple times at easyeda and their quality is quite good! Other options are PcbCart, Elecrow and iTead.

[Jbates58]

so, just to check. am i set to order it now? does it all check out from the pros?

do the manufacturers check them before, to see if there is any issues?

Jason

[pix3l]

You might want to have a look at where your traces went that connect your IP+ and IP- pins....

Have you thought about how you will program the atmegas?

[Jbates58]

You might want to have a look at where your traces went that connect your IP+ and IP- pins....

Have you thought about how you will program the atmegas?

the chips will be socketed, and programmed in another uno. will only need to flash them once.

i removed the traces, as i replaced them with the solder top layer mask. thought they were redundant. is this not a good idea?

looking at it, it wont seperate the traces on the top layer from the GND top layer. can i get away with removing the top GND? and just have the bottom layer as GND?

Jason

[pix3l]

That  won't work: your input connectors aren't connected to anything at the moment. The solder mask shape you have drawn will only mean that under the purple shape, the copper that is present there will not have any (green) solder mask "paint" on them.

Removing top GND plane is up to you, as long as you make sure that there are no "floating" GND islands that are not connected to the other parts of the GND plane.

[Jbates58]

That  won't work: your input connectors aren't connected to anything at the moment. The solder mask shape you have drawn will only mean that under the purple shape, the copper that is present there will not have any (green) solder mask "paint" on them.

isnt that what i want though? so that i can beef up the exposed copper trace with solder?

or will the exposed copper not be connected to the pads?

Jason

[pix3l]

Now I see, the purple shapes are on the topSolderLayer, I thought they were on the solder mask layer.

Looking at the "Photo View", they will be connected.

Now you removed both GND planes? Routing out all GND connections is probably not the best idea...

[Jbates58]

no, its still there. i just changed the fill style to none to hide it so i can see the traces. as it highlights the top layer stuff in red. and i cant see the wire trace links on the top layer.

so, based on thepurple section ("TopSolderLayer") do you think that will then leave pure exposed copper on the pbv? or will i still need to keep the wire trace and beef it up in width?

i have experimented, and i can get a 100mil trace in the purple section i have defined. or is that redundant?


Jason

[pix3l]

Have a look at the photo view (image attached where to click)

[fsedano]

Hello,

Why 2 uC? You have 6 ADC inputs to use, and you can multiplex 2 LCDs by using one spare pin to connect the 'E' entry from the second LCD.

If you really want to have 2 uCs for whatever reason, I'd suggest to do a board with 1 uC+ 1 LCD and just build 2 of them.. That way you can go higher or lower in the future.