LTspice problem simulating LM4562, floating nodes error

Discussion in 'General Electronics Chat' started by nidhogg_4, May 9, 2016.

  1. nidhogg_4

    Thread Starter New Member

    May 9, 2016
    4
    0
    Hi, I have been trying to simulate a simple transimpedance amplifier using the current feedback opamp LM4562 but I am getting this errors when I run the simulation:

    WARNING: Node U1:1:U11:VP1 is floating.
    WARNING: Node U1:1:14 is floating.
    WARNING: Node U1:1:U11:VP2 is floating.
    WARNING: Node U1:1:U11:VP3 is floating.
    WARNING: Node U1:1:U11:VP4 is floating.
    WARNING: Node U1:1:U11:VZ1 is floating.
    WARNING: Node U1:1:U11:VZ2 is floating.
    WARNING: Node U1:1:U11:VZ3 is floating.
    WARNING: Node U1:1:U11:VZ4 is floating.
    WARNING: Node U1:1:9 is floating.

    Direct Newton iteration failed to find .op point.
    Singular matrix: Check nodes u1:1:u11:vz2 and u1:1:u11:vz1
    Iteration No. 1
    Fatal Error: Singular matrix: check nodes u1:1:u11:vz2 and u1:1:u11:vz1
    Iteration No. 1

    This circuit has floating nodes.

    The circuit I am using is attached.

    Any ideas of how could I solve this? I looked into the model file but I don't understand it too well.

    Thank you
     
  2. eetech00

    Active Member

    Jun 8, 2013
    649
    112
    You need to specify a model file defining the opamp. Did you check the TI website?
     
  3. nidhogg_4

    Thread Starter New Member

    May 9, 2016
    4
    0
    I do have the model file and I did specified it by using .lib command. The model file I am using is attached to this response.
     
  4. eetech00

    Active Member

    Jun 8, 2013
    649
    112
    Post your LTspice .asc file please.
     
  5. nidhogg_4

    Thread Starter New Member

    May 9, 2016
    4
    0
    Attached asc file. Thank you for the help!!!
     
  6. eetech00

    Active Member

    Jun 8, 2013
    649
    112
    Hi

    I've attached a zip file with a "fixed" LM4562Fixed.LIB" file
    It should work now.

    Schematic changes:
    I used an unmodified built-in LTspice opamp2 symbol.
    I included the LM4562Fixed.LIB file.

    LM4562.LIB file changes:
    was:
    .SUBCKT LM4562 Vinm Vinp VCC VEE Vout
    changed to:
    .SUBCKT LM4562 Vinp Vinm VCC VEE Vout

    was:
    EGNDF GNDF 0 VALUE = {(V(VDD)+V(VSS))*0.5} <--this resolves to "0"
    changed to:
    EGNDF GNDF 0 VALUE = {V(VDD,VSS)*0.5}

    You should let TI know there is an error in the LM4562.LIB spice file
     
    nidhogg_4 likes this.
  7. nidhogg_4

    Thread Starter New Member

    May 9, 2016
    4
    0
    Thank you so much for the help!!!!! It works
     
Loading...