Need help Proofing a LIFEPO4 PCB

Discussion in 'The Projects Forum' started by Ladvien, Nov 13, 2012.

  1. Ladvien

    Thread Starter New Member

    Sep 29, 2012
  2. n1ist

    Active Member

    Mar 8, 2009
    Look at the schematic in figure 2 of the apps note. Your schematic has some major differences:
    - Pin 1 and Pin 2 must be connected together and to your DC bus
    - Pin 3 and Pin 4 must be connected together and to the positive of your battery and capacitor
    - Pin 8 and Pin 9 must be connected together and to ground
    - The negative of your battery must be grounded
    - You will probably need a local 4.7uF cap on the Vcc rail of each chip (or maybe every pair of chips)
    - the chip has an 11'th "pin", the heat slug, which should be grounded

    As for the PCB, there are a number of issues:
    - First of all, will you have a means of soldering a DFN package with a heat slug?
    - High current traces (ie the positive bus from the input connector, the connections to the battery) need
    to be much thicker. Look at the data sheet for the chip for a sample layout
    - The ground plane is broken up to the point of being useless. I would try to route as little as possible on that layer and try to keep it one piece. Make sure the connection between the programming resistor and ground is short, direct, and not in a high-current path
    - Traces should connect to pads or other traces at right angles. Avoid acute angles that can trap etchant (acid traps)
    - Traces should bend at 45 degree angles rather than 90 degree angles
    - The thermal pads under the chips should be grounded. They also need to be on the same side as the chips as the chips have heat slugs (external metal pads) that must be soldered to the thermal pads. They are the heat sinks for the chip. If the ground plane is on the other side of the board, I would use multiple vias to transfer the heat. These vias should be next to, not under, the chip
    - I would locate the ICs next to the battery connector and put the status LEDs and programming resistors on the other side of the ICs. Likewise, I would move the input connector to be in-line with the chips and run a thick trace across from the input connector to the ICs
    - The filter caps should be right next to the ICs. Ideally traces would connect to the cap and then to the chip, and the connections must be wide and low inductance. If the ground plane is on the other side of the board, I would use two vias to connect the caps to the plane
    - Some traces look like they are quite close to each other. I would start the design with 10/10 or 8/8 mil rules (traces at least 8 or 10 mils wide, and at least 8 or 10 mils apart from each other or other copper). You will likely have to tweak this around the chips given their size
    - You have no outline
    - You have silk screen "Name" and "Value" by the ICs. Those should be cleaned up
    - I would add the board name, revision, and your name to the top silkscreen
    - Add a pin 1 indicator on the silk to each chip and a cathode indicator to each diode

    Ladvien likes this.
  3. Ladvien

    Thread Starter New Member

    Sep 29, 2012
    I greatly appreciate the level of detail. I will make the changes.