Circuit Design problem with Capacitor

Discussion in 'The Projects Forum' started by khatus, Aug 10, 2018.

  1. khatus

    Thread Starter Member

    Jul 2, 2018
    38
    1
    Currently i am designing a PCB board for my new project. But the problem is, the chip or ic i'm using has the following connection for Supply in it's data sheet (it's common :p) the entire bottom layer is ground plane.
    [​IMG]

    Three, same type of Ic will be used for my project.I connected them with 12V supply in the following manner as shown below

    [​IMG]

    But later i thought another kind can also be used like this

    [​IMG]

    But Now I am little confused which connection should i use?? What will be the difference if i use connection-2 instead of connection-1.

    In the second connection i used a 0.3 uF capacitor with the supply. since the capacitor(0.1uF each of them) connected across VCC and ground of each individual IC's are in parallel.
    3*0.1uF = 0.3uF.

    Can Someone explain, which circuit will function properly?and why?

    NB: the ic's are IR2110 Mosfet driver.
     
  2. AlbertHall

    AAC Fanatic!

    Jun 4, 2014
    6,643
    1,553
    Connection-1 is the one to go for.
    Each chip should have the capacitor connected with the shortest possible connections. This minimises the inductance in series with the capacitor and so minimises the impedance across the chip supply pins so when the chip draws pulses of current there is minimum disturbance of the chip supply voltage.
     
    khatus likes this.
  3. ebp

    Well-Known Member

    Feb 8, 2018
    2,207
    773
    The individual capacitors should be used, each placed as close as possible to the supply pin of the IC and each with a direct connection to the ground plane. Assuming they are surface mount, probably a single via is adequate but if you need to use very small ones it might be good to use two or three per capacitor.

    Gate drivers "source" a lot of current to rapidly charge the capacitance of the FET's (or IGBT's) gate. Power distribution on a PCB always has inductance. Solid planes are very good, but individual tracks are not so good. You can't instantaneously change the current through an inductor. Without the caps, when the gate driver output goes HIGH and sources current into the gate capacitance, the sudden attempt to demand more current will make the voltage at the positive supply pin fall because of the inductance. The capacitor acts as a local charge reservoir that can supply current with only a small dip in voltage while the current through the inductance of the track "catches up." Though it doesn't usually happen with a gate driver, if the current very suddenly dropped the inductance of the track would cause the voltage to go very high - current stays constant, the load now looks like a higher resistance so by Ohm's law the voltage must go up. Now the cap acts as a local reservoir into which the inductively stored energy can be dumped. Obviously, for the cap to do its job well there must be as little inductance as possible between it and the driver.

    These "decoupling" or "bypass" capacitors sometimes need to be higher in value but sometimes can be lower, depending very much on just what the circuit does. 0.1 µF is a very common value. At that capacitance, a ceramic capacitor is almost always the best choice. I recommend "X5R" or "X7R" types because the behave better than some others. Some types have a really big negative voltage coefficient of capacitance - as the voltage across them goes up the capcitance goes down. Some are so bad that if you operate them near their rated voltage the capactance can be down to 25% or less of the nominal value. XxR types do suffer from this, but not nearly as badly as types like "Y5V" or "Z5U." XxR types are a little more expensive.
     
    Last edited: Aug 10, 2018
    khatus likes this.
  4. Darkg

    New Member

    Jun 1, 2018
    10
    0
    Not much to add. Your confusion comes from assuming that a track is simply a conductor, like an ideal conductor. Often that is a useful assumption. In this case it is not!
     
  5. crutschow

    Expert

    Mar 14, 2008
    20,216
    5,716
    I must have missed something. :confused:
    You show Vcc connected directly to ground.
    If Vcc is a plane it should not be identified with a ground symbol.
     
  6. Darkg

    New Member

    Jun 1, 2018
    10
    0
    I think everyone but you missed something. Quite right, connecting Vcc to ground is considered bad practice :rolleyes:
     
  7. Ylli

    Member

    Nov 13, 2015
    401
    103
    Also, that is not the right pinouts for a IR2110.
     
  8. khatus

    Thread Starter Member

    Jul 2, 2018
    38
    1
    ignore the ground symbol at the end of VCC rail.it was mistakenly placed during drawing
     
  9. yogesh gupta

    New Member

    Aug 11, 2018
    1
    0
    Thats Right
     
  10. ebp

    Well-Known Member

    Feb 8, 2018
    2,207
    773
    I should have mentioned:
    If the pinout of a device is such that the supply and ground pins are close together, the effectiveness of the decoupling caps can sometimes be improved by placing it between the supply and ground pins, even when planes are used for power. This may reduce inductance in the critical path by removing vias to the planes from that path.

    A great many newer datasheets and even revisions of sheets for ancient parts now include a recommended layout drawing that will include decoupling caps.
     
Loading...