This thread has been locked.

If you have a related question, please click the "Ask a related question" button in the top right corner. The newly created question will be automatically linked to this question.

LDC2114: LDC2114 Layout Example

Part Number: LDC2114

Hello,

we are currently designing multiple LDC2114 in our project.

We're currently implementing the PCB Layou and have a few questions there.

  • We are plaing to route the IN-lines in the inner layer and shield the IN-lines top and bottom with COM, like it's described in the following picture
  • But in the Layout Example of LDC2114 Datasheet COM Layer seems to be in the middle Layer and IN lines seem to be on bottom layer
  • So how should the COM Layer be routed correctly? Should it be in middle layer under LDC2114 and top and bottom later?
  • I've attached Gerber Files 

Kind regards,

Clemens

gerber.rar

  • Hi,

    Pin 1 is the return(COM) for ALL the LC tanks, and connected to the brown plane, The light cyan is the POWER GND.

    Shielding should not be connected to any of these and should be connected to the shield/drain of your interface connector. As far as how to layout out a shield plane on your board, depends on how the shield is used within the system.

    Hope this helps.
  • Hello, are you sure shielding should not be connected to COM?
    Snoa962 says clearly that signal traces should be routed on the middle layers of the PCB with a ground shield (or COM for the LDC211x) above and below.
  • Hi,

    Yes I am sure, the idea of a shield is not to reject the noise, rather guide it and/or provide a low impedance path to ground, which should be connected to the source.

    Based on this:

    Top Layer => shield flood, connected to the shield of your source connector, ie the shield on the USB cable if that is what your are using, that shield will connect to the ground of the power supply on the host (computer)

    Mid 1 => Lnx signal

    Mid 2 => Lnx GND, connected to pin 1 of the chip

    Bottom Layer => Same as top layer but should connect to top layer with vias if possible.

    If you have a shielded cable, the shield of the cable will eventually connect to ground, but at the system source,

    Hope this helps.

  • Hi,

    but why says Snoa962 to shield the IN signals with COM?

  • Hi,
    Essentially, Section 2.1.1, end of first line and before parenthesis at the begging of the second line tells you the same thing I explained to you before:

    2.1.1 Trace Shielding
    For optimal EMI performance, signal traces should be routed on the middle layers of the PCB with a
    ground shield (or COM for the LDC211x) above and below. This effectively creates a low impedance
    shield above and below the traces which helps protect against incoming and outgoing electric fields. If the
    application requires the sensors to be connected remotely by an external cable, then the cables should be
    short, shielded, and in a twisted pair whenever possible.

    You must provide a low impedance path to the unwanted signal, the author is calling it "ground shield", this would be a copper flood that connects to the shield of a connector, in this case the shell of the USB connector. If you read the specifications for such connector, there is an actual GND pin on the connections, this pin is intended for power reference and not for shielding and several pins that connect to the metal of the case, these are intended for the shield.

    The statement within parenthesis says: (or COM pin for the LDC2011), in my personal opinion, second best, once again it all depends on how the whole system connects because if the host has no shield tied to the ground at the power source, (of the host), the shield is just floating copper and potentially is drawing more noise into your system.

    Edgar.
  • Hello All,

    As Edgar mentioned, for the LDC211x devices, we recommend shielding above and below with COM. Ground shielding can still be used if there is no other option, but doing so can increase the overall noise.

    The COM shielding should be both above and below the sensor. If you have only the top or bottom shielded (with the shielding isolated by a thinner dielectric of 10mil or less), there will be a sensitivity to capacitive shifts on the INx line. If someone touches the INx trace, it could produce a capacitive shift large enough to affect sensing performance temporarily.

    The recommended layout in the LDC211x Datasheet shows the INx traces on the top layer with COM shielding underneath but without COM shielding above. For applications where it is not possible to physically touch the INx trace, this design can be acceptable. If the sensor is not integrated into the PCB, then the use of shielding on both top and bottom is recommended.

    The recommended layout shown was more focused on showing where to place the bypass and sensor caps, and also how to route the COM layer.

    Regards,

    ChrisO

  • Hello,

    thanks for your answer! I'll shield IN lines both above and below with COM
    Regards,
    Clemens