Hi Erik,
Thank you very much for your Reply, I am making changes indicated by you Here is the new list.
Techniques to reduce EMC sensitivity of system

1. Insert a soft ferrite bead like BL02RN2 (Murata) or similar where the +5V enters the board, just between power supply connector and the bulk decoupling capacitor. This will heavily minimize high frequency currents running in the power supply cable.

2. Have ferrites at the entry to a steel case with your board for all outside connections.
Have all connections to the high amperage galvanic isolated [ eg: opto isolated ] in a way that does not allow any noise from the high amperage parts enter your steel box.

3. Pay adequate attention to enclosure design. Use Mild Steel around 1mm thick with Zinc coating. Don’t have any unwanted holes or openings in the enclosure. For ventilation some tiny holes 2mm diameter can be introduced but keep the number of holes as small as possible.

4. For cables leaving or entering your enclosure tie the cable shields to the enclosure at the point where these cables enter or exit your box. All your cables must exit and enter one and the same location. Yet there must be some isolation among cables with different signal types.

5. Connect the Signal Ground and Safety ground with the enclosure at the point where your bales enter and exit the Enclosure Box.

6. It’s better if a ferrite is used to connect signal ground, enclosure ground, Safety Ground. Ferrite will act as a short when there is no noise in grounds but will effectively isolate them if there is any noise.

7. Noise entering into your box depends on the length of the holes and not on the areas. If at holes are desired make them square or circular but not rectangular.

8. If you need to connect devices like keypad or display for which a large hole is needed in the box. Use the Clean box dirty box method for incorporating these devices.

Good PCB layout Techniques

1. Keep the crystal and burden capacitor tracks shortest. Do not connect the ground pins of 33pF capacitors to ground plane. Connect them directly to microcontroller ground.

2. Do not encircle the crystal with signals. It'll couple noise to whatever you connect. Run them on the same side of the crystal. And put a shield trace between the crystal signals and those I/O. If they go any distance, consider an R/C filter (47R and 0.001 uF depending on their speed).

3. Ground-fill under the crystal might improve emissions. If you do ground-fill, it needs to be properly anchored.

4. Route solid ground planes on both sides of PCB, if you use double sided PCB do not use solid Vcc plane, but ground planes on both sides, and lot's of vias between them

5. In critical situations, especially if very high clock frequencies are used, the two burden capacitors can be soldered directly across pins of microcontroller. By this any copper traces are omitted 'by design'. The crystal is then connected by as short traces as possible.

6. It must be kept in mind, that all these currents, which flow in the crystal circuit will flow back to the ground pin of microcontroller!!! And so, there must always exist an as perfect as possible connection of involved ground pins of crystal circuit (ground pins of burden capacitors) to the ground pin of microcontroller! But not enough, also all ground return currents caused by charging of stray capacitance must be fed directly to ground pin of microcontroller. And the housing of quartz IS a source of stray capacitance, which must be grounded adequately!

7. Don’t weave tracks from your outside world through the cpu side. Not a good idea - try and maintain as much separation as possible - even to the point of using small pads on the optocoupler and don't run tracks between the optocoupler. You're wanting the opto to give you voltage isolation so don't compromise it with your pcb.

8. It can help to surround the microcontroller circuit on top layer by a guard trace (which is connected to ground plane, maybe by vias).

9. Ground plane extended over all signal traces in combination with guard trace arround certain points act as a shield, as if you have put the whole board into a metal enclosure. And this by only using a solid ground plane without making compromises!

10. Ground plane also provides a ground return current path for every signal trace next to it, and by this heaviliy minimizing created loop and as result, radiation from this signal trace and susceptibility against radiation

11. two different digital signals must always be separated by certain distance, so that toggling of one line will not propagate to other line due to charge injection via stray capacitance. If both digital lines are very close to each other and you toggle one of the lines very quickly, then you will notice a very fast spike on the other superimposed to its signal. If noise margin is violated, then you will become trouble...

12. One way to prevent such cross coupling is to shield the different signals to each other, by routing a solid ground plane between them

13. Another way to shield these signals, is to route them over a solid ground plane. But this is only helpful, when distance to solid ground plane is heavily decreased, like it is used with multilayer boards. It can be calculated, that the stray capacitance between the signals decreases to the same amount as the capacitance between signal and ground plane increases! Multilayer boards provide a very effective shielding between digital signals by this methode.

14. Sometimes it can be seen, that bus signals are routed very close to each other, even when no ground plane is very close underneath. As long as the signals belong to the same bus, where all signals are simultaneously clocked, means toggled, then a bit stray capacitance can be allowed if source impedance of drivers is very low and bus timing is not too fast. Then, injected charge due to cross coupling can be removed again before data on bus is latched.

15. If you route a digital signal over a solid ground plane, then the ground return current will always flow directly underneath the signal current, not elsewhere on the board. This is especially valid for the high frequency content of signal. It can be shown, that by this current flowing scheme resulting magnetic field is minimal. And as inductivity is defined as produced magnetic flux per current, this also results in a heavily minimized inductivity of according signal traces.

Techniques to reduce EMC radiation from system

1. It can be helpful to insert 10...47Ohm resistors at outputs of 74HC541 for cables leaving or entering board.

2. Put a soft ferrite in series with Vcc as close as possible to pin 40 of the MCU, with a dedicated filter cap between it and the MCU. On a 2-layer board this is sometimes the only way to control EMI.(Blast that 20-40 ground/power arrangement).

3. For cables carrying signals from one board to the other It's a good idea, to use a flat cable for this purpose, where each second, or at least third line is a ground line. All these ground lines MUST be connected to ground at each board!

4. Switching SSRs can produce some interference. Also, via cables to outer world interference is fed very near to your microcntroller circuit. This can make troubles! To prevent trouble, you should keep microcontroller circuitry and output side of SSRs much much farer away from each other. Sometimes, it can be helpful even to add a metal plate placed close over the micro board and connected to ground plane at several places. This metal plate will act as a shield: Every stray capacitance to the SSRs and their loads will end on this metal plate, and not inside your micro circuitry.

5. Keep the microcontroller clock & logic spped minumum just enough to run the application.

6. Use common mode filtering on cables leaving or entering the board. Otherwise it will result in heavy noise radiations. Bend each cable arround an individual soft ferrite ring core or feed it through a bigger soft ferrite bead. This will minimize common mode noise on each cable and by this minimize radiation. In any case, keep the cables as short as ever possible!!

7. Try to avoid 90 degree bends on your tracks. Using two 45 deg bends (or a radius) reduces EMI.

Erik Is it OK Now?

Regards,
Prahlad Purohit