ADUM5400 and ADUM1400 EMI issues

Hello ADI Support:

My customer is currently designing an isolated serial card using the ADUM 5400. The PCB dimensions will be the standard PC-104 card size. Along with the ADUM 5400, They will also be using the ADUM1400 to isolate other signal lines.

The isolated side will draw about 19ma on a worst case scenario from the ADUM5400. We read the AN-0971 application note and want to implement some of the techniques to reduce the emission from the IC.

However, they do not have the area to incorporate the stitching capacitor techniques. The real estate on the PCB is on the low end because they have four different isolated sections that use both the ADUM5400 and ADUM1400.

Will the emission emitted corrupt signal line if they do not incorporate the stitching capacitors?

How else can they reduce emission if none of the app note techniques can be implemented on the design?

Thank you,

Frank

  • 0
    •  Analog Employees 
    on Dec 15, 2012 1:09 AM over 8 years ago

    Hello Frank

    You will not have data corruption issues if you don't do the stitching capacitance. 

    Assuming you are not running the data channels above 5Mbps, the primary radiation issue will likely be from the isoPower.  The fact that you are running a relatively light load will help.  Will your application be in a conductive enclosure?  If so, you will get some shielding from that. 

    The stitching capacitance is the primary advice we give to customers to reduce emissions.  You can build the stitching capacitance by combining surface mount safety caps as well as the in the board stitching shown in the app note, both are required to minimixe area.  The combination of the ultra low inductance in the PCB stitching in parallel with the high inductance capacitance on the PCB will allow the combination to not take up much space on the PCB.  Make as much in PCB stitching as possible without growing the board, then supplement with safety caps until you meet your emissions goal.

    I will be happy to look at your designs if you will share the PCB layout.

    MSCantrell

  • Hello MS Cantrell,

    I don't understand what you mean by the statement," You can build the stitching capacitance by combining surface mount safety caps as well as the in the board stitching shown in the app note, both are required to minimixe area."  How are you minimizing area by adding more caps?  Do you mean that both are required to minimize EMI?

    Thank you,

    Frank

  • Hello MS Cantrell,

    I have further questions.

    The cards are going to be transmitting at 1Mbps, so hopefully it will be good. The standard product will have an enclosure, but my concerns are with the ones that order the OEM version which will not have an enclosure.

    I don't really have the room for more components, but if needed I can make the room.

    I have a few questions about the stitching capacitance and safety caps...

    Can the stitching capacitance be in a shape of a U or a donut border around the isolated area? There are four different isolated powers, so going straight down the board will not work.

    The examples on the app note just show example for straight stitching capacitor that goes down the middle. This was an example for one chip, I have four per system.

    How do I implement the safety caps? On both sides of the non isolated and the isolated side? What are the recommended values? Can I do it so I just add safety caps and no stitching?

    Thank you,

    Frank

  • 0
    •  Analog Employees 
    on Dec 17, 2012 9:03 PM over 8 years ago

    Hello Frank,

    When I say the stitching capacitance, I am referring to the whole capacitance between input and output.  It can be made up of PCB internal cpacitive stitching and dicrete capacitance mounted on the surface.  The preferred type is built into the PCB since it has the lowest inductance and the highest frequncy.  If as in your case, you have space restrictions that limit the stitchng capacitance that can be made inside the PCB, then that can be supplimented with a high voltage safety rated capcaitor across the barrier.  These are lower frequency capacitors so if you can build enough capacitance into the PCB that is the best, combining as much PCB stitching as possible and supplimenting with safety caps will work for limited space.  Using safty caps by themselves is not effective.  I would recommend a minimum of 30pF in the PCB and about 300pF total capacitance across the barrier.  I have had customers use up ti 1nF on the surface for high power applications.

    The stitching capacitance in the PCB can be any geometry and can follow the top layer creepage zones.  U shapes and even rings will work.

    Make the internal stitching capacitance between ground planes and the planes that supply power to the isoPower device.  Any plane will be useful, since they are all the same from an AC point of view, but the planes that carry the current will be the best.

    Safety caps are just a high voltage safety rated capacitor. Johanson or Murata supply them.  Johanson has the surface mount versions and good documentation on how to use them. 

    www.johansondielectrics.com

    I hope this makes it clearer.

    MSCantrell

  • Hello MS Cantrell,

    This does make it clearer and I do have a few more questions.

    I just implemented the stitching capacitance and got it to about 35pF. I have include a picture of the one side that I just laid out. The blue outline is the PWR cutout and the white outline is the GND cutout.

    Comments?

    Can you elaborate on the safety capacitors? When I have the capacitor across the gap (barrier), what do I connect it too?

    Regular GND and ISO GND?

    Regular PWR and ISO PWR?

    Both?

    Floating?

    It is similar to a floating stitching capacitance structure where its not connected to anything? So instead of it internal to the PCB its on the outer layers?

    Thanks for the help. It has really been helpful.

    Frank