Can you give us a schematic also?

1. Ok, like others already said, you must provide much wider distances at the relay contacts!!!!!!!!! What you do with the mains routing there is illegal!! You cannot route mains traces in such a close distance to each other. I guess there's a lot of arcings when the relay contacts open??? Maybe this is already the cause of your malfunctionings!

2. Also illegal is the distance between mains and drive contacts! At least 8mm should be provided here. Avoid ground fill here!!! The gap must be absolutely "copper-free".

3. You connect signals to the board, that are not filtered. For instance the input voltage of 5V regulator, connected to "RConn", can unmolestedly run across the whole board. If EMI like high frequency interference or ESD is hitting this line, then it must interfere the whole board!

4. A major mistake of your board is, that cables leave it at different, yes even opposite locations. These means, that any EMI that is coupled into a cable can run across the whole board! This can even be problematic with a mulitlayer board containing a solid ground plane. But with a double sided board this is deadly.

Assume for instance, that you have connected a RS485 cable which sees at its other end a good connection to ground or earth potential. Now let one of the relay contacts receive EMI from mains (even only the openings of contacts is EMI enough), then you have a considerable EMI current running over your entire board! Don't think, that the relay and related optos really provide any serious isolation. There's so much stray capacitance that still enough EMI is running over your board.

This is a very nasty mistake, because it only becomes perceivable, when EMI is there. So, this is a product working perfectly on your living room desk, but starts to make trouble in industrial environment.

Better is, to move all cables to one location of board, so that this kind of "across board running" cannot take place. Of course, to make this properly work, you need filtering right where the cables enter your board, where all this filtering is referenced to a local ground plane, better called radio frequency plane, so that all this noise cannot go further than this cable entry point! Better is to additionally use shielded cables, and to connect the cable shields to this radio frequency plane too.
Best is to make this radio frequency plane part of your enclosure. But you can also use your one and only ground plane for it, as long as you only use the region nearest to the edge of board for it.

5. You need proper supply voltage decoupling at EACH chip. A 100nF/X7R at each chip is a must! Also, supply voltage decoupling cannot work properly without solid ground plane!
For the same reason, don't use the 8052 in DIL40 package. This package is difficult to decouple. Use at least PLCC44 package. I always use TQFP44 package in combination with ISP programming.

More I can say only when having a schematic.

Kai