• State TI Thinks Resolved
  • Locked Locked
  • Replies 3 replies
  • Answers 1 answer
  • Subscribers 39 subscribers
  • Views 800 views
  • Users 0 members are here
Support feedback
Options
Options
Similar topics

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.

PSPICE-FOR-TI: Cadence Inductor Pspice library & (ORPSIM-15256) not a subcircuit param

Anders Dunkars
Intellectual 1130 points
Part Number: PSPICE-FOR-TI

Im trying to use Coilcraft Inductor models with PSpice-For-TI

https://www.coilcraft.com/en-us/models/howto/model-libraries-for-pspice/

but I get strange simulation results that may relate to the following warnings: 

Reading and checking circuit
WARNING(ORPSIM-15256): <X_U3.X1.L_F0> not a subcircuit param
WARNING(ORPSIM-15256): <X_U3.X1.L_EL> not a subcircuit param
WARNING(ORPSIM-15256): <X_U3.X1.L_Z0> not a subcircuit param
WARNING(ORPSIM-15256): <X_U3.X1.a> not a subcircuit param
WARNING(ORPSIM-15256): <X_U3.X1.Is> not a subcircuit param
WARNING(ORPSIM-15256): <X_U3.X1.L> not a subcircuit param
Computing impulse response for X_U3.X1.G_Rvar2...
WARNING(ORPSIM-15171): 41.0058 percent of X_U3.X1.G_Rvar2 impulse response is non-causal.
41.0058 percent of X_U3.X1.G_Rvar2 impulse response is non-causal.

Does anyone have any clue to why the tool is not accepting the sub circuit parameters - see model for U3 below 

Regards,

Anders

*======================================================================
* SPICE Model generated by Coilcraft
* Coilcraft Part Number : XEL5020-102
* Inductance = 0.95uH
*======================================================================
* Model Parameters:
* Valid Frequency Range = 0.0001GHz-0.2GHz
* Ambient Temperature = 25 degC
* DC Bias Current = 0 A
* Non-Linear Frequency Dependent Approximation
*======================================================================
.subckt XEL5020-102 port1 port2 PARAMS: Cpar=8.8pF Ind=0.95uH
X1 port1 port2 Model1A PARAMS:
+ R1=0.01
+ R2=0.0126
+ C= {Cpar}
+ K1=0.00001
+ K2=0.26
+ K3= {Ind}
+ K4=0.0001
+ K5=0.01
+ L=9.9111E-07
+ Is=33.5883694
+ a=0.62058399
+ L_Z0=0
+ L_EL=0
+ L_F0=0E6
.ends XEL5020-102

  • 0
    TI__Mastermind 32035 points

    HI Anders,

    Would you please share the entire model file?

    Thanks,
    JC

  • 0 in reply to Anders Dunkars
    TI__Mastermind 32035 points

    Hi Anders,

    X1 calls the subcircuit "Model1A" which defines 8 parameters:

    .subckt Model1A Lin Lout PARAMS:
    + R1=1
    + R2=1
    + C=1
    + K1=1
    + K2=1
    + K3=1
    + K4=1
    + K5=1
    R2 N001 Lin {R2}
    R1 Lout N002 {R1}
    C1 N002 N001 {C}
    G_Rvar2 N001 Lout LAPLACE { V(N001, Lout) } {1/K2/(-S*S/4/PI^2)^0.25}
    G_Rvar1 N001 N003 LAPLACE { V(N001, N003) } {1/K1/(-S*S/4/PI^2)^0.25}
    G_Lvar N003 Lout  LAPLACE { V(N003, Lout) } {1/(S*1e-6*({K3*1e6}-({K4}*LOG({K5}*(sqrt(-S*S)/(2*pi))))))}
    *This large resistance to ground has been added to prevent a floating node error
    R3 N003 0 100Meg
    .ends Model1A
    The last 6 parameters passed by X1 are not defined by Model1A, hence they are ignored.
    The Last warning indicates that there might be a problem with the device which is defined by a transfer function.
    Please check with CoilCraft.
    Regards,
    JC