TPSI3050: Simulation failure

A.M.

Part Number: TPSI3050

Hi,

I'm considering TPSI3050 to use as a SSR as a switch to send AC sine signals.

I want to simulate TPSI3050 from SLVMDL0F.ZIP downloaded from TI website with Orcad capture version 17.2 2016 but when I lauch the simulation I get several errors as shown below:

**** RESUMING tpsi3050_tb.cir ****
.END

INFO(ORPSIM-15423): Unable to find index file tpsi3050.ind for library file tpsi3050.lib.

INFO(ORPSIM-15422): Making new index file tpsi3050.ind for library file tpsi3050.lib.
*****************************************************************************
* (C) Copyright 2023 Texas Instruments Incorporated. All rights reserved.
* TI Confidential - Selective Disclosure
*****************************************************************************
** This model is designed as an aid for customers of Texas Instruments.
** TI and its licensors and suppliers make no warranties, either expressed
** or implied, with respect to this model, including the warranties of
** merchantability or fitness for a particular purpose. The model is
** provided solely on an "as is" basis. The entire risk as to its quality
** and performance is with the customer
*****************************************************************************
* PSpice Model Editor - Version 17.4.0
*$
.SUBCKT MODE_SEL_FUNC DUTY SEL0 SEL1 SEL2 SEL3 SEL4 SEL5 SEL6 VSSP
E_SEL0 SEL0 0 VALUE = {IF ( ((V(DUTY)-V(VSSP)) < 532mV & (V(DUTY)-V(VSSP))>= 253mV) | ((V(DUTY)-V(VSSP)) < 253mV) |((V(DUTY)-V(V
$
ERROR(ORPSIM-16366): Line too long. Limit is 132 characters.
E_SEL1 SEL1 0 VALUE = {IF ( (V(DUTY)-V(VSSP)) < 652mV & (V(DUTY)-V(VSSP)) >= 532mV, 3.5, 0)}
E_SEL2 SEL2 0 VALUE = {IF ( (V(DUTY)-V(VSSP)) < 770mV & (V(DUTY)-V(VSSP)) >= 652mV , 3.5, 0)}
E_SEL3 SEL3 0 VALUE = {IF ( (V(DUTY)-V(VSSP)) < 888mV & (V(DUTY)-V(VSSP)) >= 770mV, 3.5, 0)}
E_SEL4 SEL4 0 VALUE = {IF ( (V(DUTY)-V(VSSP)) < 1.014V & (V(DUTY)-V(VSSP)) >= 888mV, 3.5, 0)}
E_SEL5 SEL5 0 VALUE = {IF ( (V(DUTY)-V(VSSP)) < 1.183V & (V(DUTY)-V(VSSP)) >= 1.014V, 3.5, 0)}
E_SEL6 SEL6 0 VALUE = {IF ( (V(DUTY)-V(VSSP)) < 1.665V & (V(DUTY)-V(VSSP)) >= 1.183V, 3.5, 0)}
.ENDS MODE_SEL_FUNC
***********************************************************************************
* PSpice Model Editor - Version 17.4.0
*$
.SUBCKT MODE_SELECT VSSP VDDP OOK 2PIN_MODE EN2PIN RESETZ SEL0 SEL1 SEL2 SEL3 SEL4 SEL5 SEL6 SELQ0 SELQ1 SELQ2 SELQ3 SELQ4 SELQ5 SELQ
$
ERROR(ORPSIM-16366): Line too long. Limit is 132 characters.
E_TON TON VSSP VALUE = { IF (V(SEL0) > 0.5V, 140.8mV, IF (V(SEL1) > 0.5V, 300.8mV, IF (V(SEL2) > 0.5V, 460.8mV,
+ IF (V(SEL3) > 0.5V, 620.8mV, IF (V(SEL4) > 0.5V, 780.8mV, IF (V(SEL5) > 0.5V, 920.8mV, IF (V(SEL6) > 0.5V, 1080.8mV, 0V)))))))}
G_IEN IEN VDDP VALUE = { IF (((V(EN2PIN) > 0.5V) & (V(OOK) < 0.5V) & (V(RESETZ)-V(VSSP) > 0.5V)), (IF (V(SELQ0) > 0.5V, 1.9mA,
$
ERROR(ORPSIM-16366): Line too long. Limit is 132 characters.
+ IF (V(SELQ2) > 0.5V, 4.0mA, IF (V(SELQ3) > 0.5V, 5.0mA, IF (V(SELQ4) > 0.5V, 6.0mA, IF (V(SELQ5) > 0.5V, 7.0mA, IF (V(SELQ6) > 0.5
$
ERROR(ORPSIM-16366): Line too long. Limit is 132 characters.

Index has 71 entries from 1 file(s).

.SUBCKT MODE_SEL_FUNC DUTY SEL0 SEL1 SEL2 SEL3 SEL4 SEL5 SEL6 VSSP
E_SEL0 SEL0 0 VALUE = {IF ( ((V(DUTY)-V(VSSP)) < 532mV & (V(DUTY)-V(VSSP))>= 253mV) | ((V(DUTY)-V(VSSP)) < 253mV) |((V(DUTY)-V(V
$
ERROR(ORPSIM-16366): Line too long. Limit is 132 characters.

ERROR(ORPSIM-15108): Subcircuit MODE_SELECT used by X_U1.X_U1_UPRIM_UMODE_U285 is undefined

Please, could you explain how can I simulate with the library downloaded from TI? Should I modify something from the library?

Thank you in advance

over 2 years ago

0 Tilden Chen over 2 years ago

TI__Expert 8321 points

Hello A.M,

Thanks for reaching out to our team on E2E! Unfortunately, there are subcircuit conflicts between our TPSI305x-Q1 model and the TI model library. The current workaround is to remove nom_pspti.lib* from the Configuration Files before simulating.

Best regards,
Tilden Chen

Solid State Relays | Applications Engineer

0 A.M. over 2 years ago in reply to Tilden Chen

Prodigy 110 points

Hi Tilden,

Thank you very much for your help.

I removed nom.lib from the Configuration files but I sitll have errors when I try to simulate. Please find attached the errors in the output file from simulation.

2311.TPSI3050_TB_out.txt

As I'm not able to simulate the device for my application. Please could you tell me if TPSI3050 could be used as a SSR with two MOSFETs back-back in steady state performance. I mean, if EN is maintained during a long time, would TPSI3050 suitable for my application?

Thank you in advance.

Best regards

AM.

0 Tilden Chen over 2 years ago in reply to A.M.

TI__Expert 8321 points

Hello A.M,

You can keep nom.lib, please remove nom_pspti.lib* from the Configuration Files before simulating. TPSI3050-Q1 can absolutely be used with back-to-back MOSFETs, this is what we have on our EVM. However, in PSpice I would suggest modelling the MOSFET(s) as a capacitor. More details can be found below.

How to Simulate TPSI305x-Q1 and Behavior Driving MOSFET Using PSpice for TI

Sometimes it can be challenging to simulate devices models in PSpice For TI given all the different buttons and knobs. The intent behind this post is to guide the reader on how to simulate the TPSI305x-Q1 models in PSpice For TI to aid the design-in process. The following assumes PSpice For TI is already installed.

Opening TPSI305x-Q1 Model in PSpice For TI

Download TPSI305x-Q1 PSpice Model (SLVMDV1C.ZIP) and Calculation Tool (SLVRBI9) from product page.
Run PSpice For TI and open TPSI305x-Q1 testbench.

Determining CVDRV, CDIV1, and CDIV2

Select MOSFET and determine total gate charge from datasheet for sizing load capacitor (CVDRV) in testbench. In this example, we use UJ4C075060K3S from the EVM.
Total gate charge = 37.8 nC
CVDRV=Q/V
CVDRV=37.8 nC/15 V (would use 10-V for TPSI3050-Q1)
CVDRV=52 nF
Determine CDIV1 and CDIV2 using Calculation Tool (SLVRBI9)
Set CDIV1, CDIV2, and CVDRV values in testbench. For the sake of realistic capacitances, CDIV1=10 nF, CDIV2=33 nF