Help needed in 4 channel SSR Relay schematic

Thread Starter

saqeb

Joined Nov 21, 2022
9
Hi friends,

I am a software engineer and there is a requirement to build a custom 4-channel relay PCB. I have designed a PCB but I am a bit confused about connecting SSR INPUT PINS (polarity). Can anyone of you help me? I will use this relay PCB for arduino compatible ARM I Just want to make sure before fabrication and SMT that nothing is wrong. Sorry if I fail to elaborate my problem clearly.

https://oshwlab.com/saqeb/relay-test
 

ronsimpson

Joined Oct 7, 2019
2,527
Please post an athematic.
Relay part number https://media.digikey.com/pdf/Data Sheets/Omron PDFs/G3MB.pdf
There are two filled areas on the PCB. Ground and supply?

The diode across the relay input is not needed with a SS relay.

The copper area "ground & supply" should be increased to the left to include the input connectors. Extend to the left almost to the edge of the PCB. The grounds in that area are week.

I don't know what voltage the relays are driving but I think power line voltages. The spacing is too small! Near the output connectors the copper is almost touching copper.
1669039581847.png

1669039607470.png
You need more space in these places.
1669039752670.png
 
Last edited:

ronsimpson

Joined Oct 7, 2019
2,527
I updated my comments above. You might have to refresh to see the changes.
I do not understand why the "MOV"? The output connector, MOV, relay and back to the connector, I do not understand. I think the MOV should be across the relay not in series with it.
 

MrChips

Joined Oct 2, 2009
27,679
Examine every trace and make sure that they flow nicely horizontally and vertically while being well spaced away from each other and other pads. Check to see if there is a different way of routing each trace. See if the trace can be routed on the bottom layer instead of the top layer.

I don't see any need for flood planes for this application.

PCB layout is called "artwork". Thus it should be your piece of art that you can stand back and pat yourself on the back for creating a beautiful piece of art.

It would help if you posted the schematic diagram.

1669040294076.png
 

Thread Starter

saqeb

Joined Nov 21, 2022
9
Please post an athematic.
Relay part number https://media.digikey.com/pdf/Data Sheets/Omron PDFs/G3MB.pdf
There are two filled areas on the PCB. Ground and supply?

The diode across the relay input is not needed with a SS relay.

The copper area "ground & supply" should be increased to the left to include the input connectors. Extend to the left almost to the edge of the PCB. The grounds in that area are week.

I don't know what voltage the relays are driving but I think power line voltages. The spacing is too small! Near the output connectors the copper is almost touching copper.
View attachment 281144

View attachment 281145
You need more space in these places.
View attachment 281146
Dear Ronsimpson.

I am really very thankful for your detailed reply. I will remove the diode between relays. Again I am thankful and best wishes for such an active community.
 

Thread Starter

saqeb

Joined Nov 21, 2022
9
Examine every trace and make sure that they flow nicely horizontally and vertically while being well spaced away from each other and other pads. Check to see if there is a different way of routing each trace. See if the trace can be routed on the bottom layer instead of the top layer.

I don't see any need for flood planes for this application.

PCB layout is called "artwork". Thus it should be your piece of art that you can stand back and pat yourself on the back for creating a beautiful piece of art.

It would help if you posted the schematic diagram.

View attachment 281148
Thanks for your valuable comments.
 

ronsimpson

Joined Oct 7, 2019
2,527
There should be a capacitor from supply to ground on the board. I might use four 0.1uF capacitors.
You can never go wrong with too much ground.
1669042393620.png
Please post your next layout.
 

ronsimpson

Joined Oct 7, 2019
2,527
One option if to place a single capacitor from supply (blue) to ground (red) right of the input connectors and left of the small parts. Because you have good grounds a single capacitor will be fine. Normally I add a small capacitor near each transistor.
 

Thread Starter

saqeb

Joined Nov 21, 2022
9
One option if to place a single capacitor from supply (blue) to ground (red) right of the input connectors and left of the small parts. Because you have good grounds a single capacitor will be fine. Normally I add a small capacitor near each transistor.
Hi Ronsimpson,

I am very thankful for your valuable comments and advice. I have redesigned and shared the schematic for your kind review. Thanks in advance.

https://easyeda.com/editor#id=|0167615896994ea48c8f0886852af08b
 

ronsimpson

Joined Oct 7, 2019
2,527
There needs to be a resistor with the "power LED".

Why D1,2,3,4? What is the supply voltage?
Looks good. Did you increase the spacing between traces at the output connectors?
 

panic mode

Joined Oct 10, 2011
2,363
very messed up and confusing thread....

1. why not post actual image of the schematic and PCB in the forum posts? having links and then changing linked content makes the thread unreadable.
2. schematics shows missing relay
1669212148372.png
3. schematics shows circuit using PNP transistor but mentioned BC547B is an NPN
4. why pass traces through SMD components? moving something slightly may completely remove need for any such 'crossing'
1669212336790.png

5. trace are passing way too close to other traces, vias and solder pads, specially in the AC section. is there a DRC in that EDA? why not setup design rules to ensure needed clearance?
1669213424673.png

6. what do you think is a reason that relay output contacts are spaces so much further apart? it is because for high voltage circuit you NEED big clearances...
1669214184261.png
so... do you know how to measure? how about keeping at least 4mm between two traces in AC section?
so ... how about something like this:
1669213357786.png

7. where are the component identifiers in the silkscreen? who can tell where the R1,R2 etc are?
8. what is the DIP4 product? an optocoupler? where is it in schematics?
 
Last edited:

Thread Starter

saqeb

Joined Nov 21, 2022
9
There needs to be a resistor with the "power LED".

Why D1,2,3,4? What is the supply voltage?
Looks good. Did you increase the spacing between traces at the output connectors?
The supply voltage is 5v, should I place a resistor for LED?
The input signal is 3.3v (Arduino like board) so I place diode (S8550-PNP). Load will be AC 22V 1A
I am sorry for incomplete information.
 

Thread Starter

saqeb

Joined Nov 21, 2022
9
very messed up and confusing thread....

1. why not post actual image of the schematic and PCB in the forum posts? having links and then changing linked content makes the thread unreadable.
2. schematics shows missing relay
View attachment 281261
3. schematics shows circuit using PNP transistor but mentioned BC547B is an NPN
4. why pass traces through SMD components? moving something slightly may completely remove need for any such 'crossing'
View attachment 281262

5. trace are passing way too close to other traces, vias and solder pads, specially in the AC section. is there a DRC in that EDA? why not setup design rules to ensure needed clearance?
View attachment 281268

6. what do you think is a reason that relay output contacts are spaces so much further apart? it is because for high voltage circuit you NEED big clearances...
View attachment 281270
so... do you know how to measure? how about keeping at least 4mm between two traces in AC section?
so ... how about something like this:
View attachment 281267

7. where are the component identifiers in the silkscreen? who can tell where the R1,R2 etc are?
8. what is the DIP4 product? an optocoupler? where is it in schematics?
I am sorry, I will post actual image of schematic.
1669215625499.png
 

MaxHeadRoom

Joined Jul 18, 2013
26,278
Those boards appear almost identical to the Opto22 line, they are available all over the net, ebay etc.
I just got rid of boxes of them that I no longer had a use for.
You can get all kinds of I/O configurations, including those that work at logic level and 24vdc.
Both AC and DC Input/output. Various boards sizes to accommodate 4,8,16,24 modules. including relay as well as SS.
They come fused together with status LED.
If you do want to make up your own boards, Opto22 have the engineering specs.
 

panic mode

Joined Oct 10, 2011
2,363
Opto22 is a good example. if making own, check other designs (even if not solid state).
note wider traces for relay output, greater clearance between output tracks and cuts in board when distance is not sufficient

1669224730807.png
 
Top