I found an issue while trying to use the TPS2597x_trans Pspice model and a potential solution:
I imported the model into Pspice for TI as the TPS2597x model is not in the TI library in the tool. When I tried to run a simulation, the sim aborted with an error reporting that component X_U7_U27 had a misalignment on the number of interfaces. Looking at the TPS2597x_trans.lib file for X_U7_U27 I see the following:
E_U7_ABM2 U7_N01391 0 VALUE { IF(V(U7_PW_IN) >= 0.93772,1,0) }
V_U7_V47 U7_N34715 0 5.469V
X_U7_U27 U7_N36070 U7_N35399 U7_N35205 $G_DPWR $G_DGND OR2
R_U7_R54 U7_N34191 U7_N34099 6.363E-01 TC=0,0
C_U7_C52 U7_N34007 U7_N33823 3.307E-03 TC=0,0
The power supply pins of X_U7_U27 OR gate ($G_DPWR and $G_DGND) are not connected to anything in the library file. This is probably the reason for the simulation error.
I also noticed that all the other OR gates in this file have a different component type and parameter settings. Here’s one example:
X_U1_U9 U1_OV_OK OVC U1_OV_B OR2_BASIC_GEN PARAMS: VDD=1 VSS=0
+ VTHRESH=500E-3
So I modified the X_U7_U27 line in the library file to follow this OR gate description:
X_U7_U27 U7_N36070 U7_N35399 U7_N35205 OR2_BASIC_GEN PARAMS: VDD=1 VSS=0
+ VTHRESH=500E-3
With this change, the Pspice model would simulate as expected.
Questions:
1. Is my modification the right way to correct this model?
2. Will the TPS2597x Trans model be added to the Pspice for TI library?
