How to run LM5046 PSPICE simulation model?

Jerome Shin

Prodigy 100 points

Other Parts Discussed in Thread: LM5046, LM258, TINA-TI

LM5046's PSPICE simulation model seems not running.

I found similar questions in E2E, but, there was no right answer.

previous answer for same question was add librarys as Global, but, the result was same.

Please help me to solve this problem.

And, would you let me know how can I convert the PSPICE model to TINA model?

My customer wants to simulate it with TINA.

※ For your reference, following is the error message (xxx.out)

**** 08/17/16 17:45:10 ***** PSpice 16.6.0 (October 2012) ***** ID# 0 ********

** Profile: "Example Circuit1-bb" [ c:\lm5xxx\3\lm5046-PSpiceFiles\Example Circuit1\bb.sim ]

**** CIRCUIT DESCRIPTION

******************************************************************************

** Creating circuit file "bb.cir"
** WARNING: THIS AUTOMATICALLY GENERATED FILE MAY BE OVERWRITTEN BY SUBSEQUENT SIMULATIONS

*Libraries:
* Profile Libraries :
* Local Libraries :
.LIB "../../../lm5046-pspicefiles/lm5046.lib"
.LIB "c:/lm5xxx/lm5046example.lib"
.LIB "c:/lm5xxx/lm5046example2.lib"
.INC "../../../lm5046-pspicefiles/lm5046.inc"
* From [PSPICE NETLIST] section of C:\Users\a0967846\AppData\Roaming\SPB_Data\cdssetup\OrCAD_PSpice/16.6.0/PSpice.ini file:

**** INCLUDING lm5046.inc ****
*In case you encounter a convergence problem, please try the simulationtion option settings as follows
*.OPTIONS ABSTOL= 1E-10
*.OPTIONS RELTOL= 0.001
*.OPTIONS VNTOL= 0.1m
*.OPTIONS ITL4= 500

*Default simulation options
.OPTIONS ABSTOL= 0.01u
.OPTIONS RELTOL= 0.001
.OPTIONS VNTOL= 10u
.OPTIONS ITL4= 100

.OPTIONS CHGTOL= 0.1p
.OPTIONS GMIN= 1.0E-11
.OPTIONS ITL1= 150
.OPTIONS ITL2= 20
.OPTIONS PIVREL= 1.0E-3
.OPTIONS PIVTOL= 1.0E-13

**** RESUMING bb.cir ****
.lib "nom.lib"
.stmlib "C:\LM5xxx\LM5046EXAMPLE.lib"
.stmlib "C:\LM5xxx\LM5046EXAMPLE2.lib"
.stmlib "C:\LM5xxx\LM5046EXAMPLE3.lib"
.stmlib "C:\LM5xxx\LM5046.LIB"

*Analysis directives:
.TRAN 0 1000ns 0
.OPTIONS ADVCONV
.PROBE64 V(alias(*)) I(alias(*))
.INC "..\Example Circuit1.net"

**** INCLUDING "Example Circuit1.net" ****
* source LM5046
C_Css         SS 0 4.7n IC=0
R_Rcs3         CS2 0 10k
C_Cbst2         HS2 BST2 0.1u IC=0
D_Dbst1         VCC BST1 DNOM
D_Dbst2         VCC BST2 DNOM
C_Csssr         SSSR 0 470p IC=0
C_Cres         RES 0 1n IC=0
C_Cref         REF 0 1u IC=0
C_Cvcc         VCC 0 1u IC=0
C_Ccs         CS 0 100p IC=0
R_Rt         RT 0 50k
D_Dcs         CS2 CS1 DNOM
R_Rdummy1         SLOPE RAMP 1m
V_Vsupply         VSUPPLY 0
+PWL 0 0 0.01m 0 0.2m 36 1.2m 75 2.2m 75 2.5m 36 3m 0
R_Rwire1         VSUPPLY1 VSUPPLY2 1m
R_Rd1         RD1 0 80k
X_F_currentXfmr    VSUPPLY VSUPPLY1 0 CS2 Example_Circuit1_F_currentXfmr
R_Rcs1         CS1 0 15
R_Rcs2         CS1 CS 499
R_Rd2         RD2 0 40k
R_Rdummy2         SSOFF 0 1k
R_Rramp         CS RAMP 15k
R_Ruv1         VSUPPLY UVLO 100k
M_M3         VSUPPLY2 HO2 HS2 HS2 NMOSNOM
X_U5B         REF_SEC FB P7V N7V COMP_SEC LM258
V_N7V         0 N7V 7
R_Rbias         COMP_SEC N16934950 2k
C_Ccomp1         FB COMP_SEC 47p IC=0
C_Ccomp2         FB CP 3300p IC=0
R_Rcomp1         COMP_SEC CP 18k
V_P7V         P7V 0 7
V_REF         REF_SEC 0 1.2
X_U8_ext         P7V N16934950 REF COMP PS2501 PARAMS: REL_CTR=1
R_Ruv2         UVLO OVP 2.6k
R_Ruv3         OVP 0 1.6k
M_M4         HS2 LO2 0 0 NMOSNOM
R_Rwire2         VSUPPLY VIN 1m
M_M1         VSUPPLY2 HO1 HS1 HS1 NMOSNOM
M_M2         HS1 LO1 0 0 NMOSNOM
C_Cbst1         HS1 BST1 0.1u IC=0
X_U6         UVLO OVP RAMP CS SLOPE COMP REF RT RD1 RD2 RES SS SSSR SSOFF HS2
+ HO2 BST2 SR2 LO2 VCC LO1 SR1 BST1 HO1 HS1 VIN LM5046
X_U7         HS1 HS2 CHB VOUT1 VOUT1 N16942154 TX1P2S PARAMS: NP=9 NS=1
L_Lpri1         HS1 HS2 240u
C_Cout1         VOUT 0 680u IC=0
L_Lout3         VOUT1 VOUT 1.6u
R_Rfbtop1         VOUT FB 25.5k
R_Rfbbot1         FB 0 15k
R_Rload1         VOUT_LOAD 0 0.11
R_Rwire9         VOUT VOUT_LOAD 1m
M_M10         CHB SR2 0 0 NMOSNOM
M_M12         N16942154 SR1 0 0 NMOSNOM

.subckt Example_Circuit1_F_currentXfmr 1 2 3 4
F_F_currentXfmr 3 4 VF_F_currentXfmr 0.01
VF_F_currentXfmr 1 2 0V
.ends Example_Circuit1_F_currentXfmr

**** RESUMING bb.cir ****
.END

INFO(ORPSIM-15423): Unable to find index file lm5046.ind for library file lm5046.lib.

INFO(ORPSIM-15422): Making new index file lm5046.ind for library file lm5046.lib.
+(V(MskPWM)<=2.5))) | (V(ILIM)>0.5 & V(PH)<=2.5),5,0) }
Etc6         TC13 0 VALUE { if(V(comp2pwm)>0 & (V(MskPWM)>2.5 | V(PH)<=2.5) & (V(delayDRVC)>0.5 & V(delayDRVC)<=2.5),5,0) }
Etc7         TC16 0 VALUE { if(V(RSTout)>2.5 | (((V(PH)>4.5 ) & (V(MskPWM)>(V(dMskPWM)+0.1)))|((V(PH)<=(V(dPH)-0.1)) &
+(V(MskPWM)<=2.5))) | (V(ILIM)>0.5 & V(PH)>2.5),5,0) }
Etc8         TC18 0 VALUE { if(V(comp2pwm)>0 & (V(MskPWM)>2.5 | V(PH)>2.5 ) & (V(delayDRVD)>0.5& V(delayDRVD)<=2.5),5,0) }

Gdd1 0 DELAYDRVA VALUE { if((V(MskPWM)<=2.5 & V(PH)>2.5) & V(VREFuv) <=2.5,1000E-12/(0.75E-6*V(RD1)-100E-9),-3.4E-3) }
Gdd2 0 DELAYDRVB VALUE { if((V(MskPWM)<=2.5 & V(PH)<=2.5) & V(VREFuv) <=2.5,1000E-12/(0.75E-6*V(RD1)-100E-9),-3.4E-3) }

Sdd6    DELAYDRVC V5V DELAYDRVC V5V SWCLAMP
Gdd3    0 DELAYDRVC VALUE { if((V(MskPWM)<=2.5 & V(PH)>2.5) & V(VREFuv) <=2.5,1000E-12/(0.75E-6*V(RD1)-100E-9),-1000E-12/(0.75E-6*V(R
$
ERROR(ORPSIM-16366): Line too long. Limit is 132 characters.
Cdd3    DELAYDRVC 0 40p IC=0
Sdd5    0 DELAYDRVC 0 DELAYDRVC SWCLAMP

Sdd8 DELAYDRVD V5V DELAYDRVD V5V SWCLAMP
Gdd4 0 DELAYDRVD VALUE { if((V(MskPWM)<=2.5 & V(PH)<=2.5) & V(VREFuv) <=2.5,1000E-12/(0.75E-6*V(RD1)-100E-9),-1000E-12/(0.75E-6*V(
$
ERROR(ORPSIM-16366): Line too long. Limit is 132 characters.

Index has 2 entries from 1 file(s).
+(V(MskPWM)<=2.5))) | (V(ILIM)>0.5 & V(PH)<=2.5),5,0) }
Etc6         TC13 0 VALUE { if(V(comp2pwm)>0 & (V(MskPWM)>2.5 | V(PH)<=2.5) & (V(delayDRVC)>0.5 & V(delayDRVC)<=2.5),5,0) }
Etc7         TC16 0 VALUE { if(V(RSTout)>2.5 | (((V(PH)>4.5 ) & (V(MskPWM)>(V(dMskPWM)+0.1)))|((V(PH)<=(V(dPH)-0.1)) &
+(V(MskPWM)<=2.5))) | (V(ILIM)>0.5 & V(PH)>2.5),5,0) }
Etc8         TC18 0 VALUE { if(V(comp2pwm)>0 & (V(MskPWM)>2.5 | V(PH)>2.5 ) & (V(delayDRVD)>0.5& V(delayDRVD)<=2.5),5,0) }

ERROR(ORPSIM-15108): Subcircuit TX1P2S used by X_U7 is undefined

over 9 years ago

0 Britt Brooks - Online Design Tools over 9 years ago

TI__Mastermind 41310 points

Jerome,

There are several issues that need to be corrected. First, the lines that are too long must be updated. I split the lines in the .lib file. It is attached below.

lm5046.lib

Next, since this is a very old PSpice design, you would need to convert it to the version you are using (16.6). PSpice should do this for you automatically, however, you will still need to create a .sim profile for the design. Once you have done that, you will need to add the nom.lib file to your include files to access the devices that are built into PSpice. After you have done all of these steps, the simulation runs properly.

Here is a .zip file with the changes I made that you should be able to use as well.

LM5046_Example.zip

There are two example circuits that should run for you in this zip file.

Since the PSpice model is unencrypted, you should be able to directly import it into TINA-TI using the New Macro Wizard.

0 Jerome Shin over 9 years ago in reply to Britt Brooks - Online Design Tools

TI__Prodigy 100 points

Hello Britt,

Thank you for your answer.

I've tryied to run the model that you shared, but, it also didn't work.

It looks have some library problem, but I can't modify it.

regarding converting the design to TINA, it also showed error on New Macro Wizard.

(Missing syntax element. Line:#347. XDFF1 DFF2 DFF3 DFF4 DFF5 RSFF5K PARAMS:)

If you can convert PSPICE model to TINA, please share the converted TINA model.

following is the error message.

**** 08/24/16 10:37:59 ***** PSpice 16.6.0 (October 2012) ***** ID# 0 ********

** Profile: "Example Circuit1-a" [ c:\lm5xxx\2\lm5046-PSpiceFiles\Example Circuit1\a.sim ]

**** CIRCUIT DESCRIPTION

******************************************************************************

** Creating circuit file "a.cir"

** WARNING: THIS AUTOMATICALLY GENERATED FILE MAY BE OVERWRITTEN BY SUBSEQUENT SIMULATIONS

*Libraries:

* Profile Libraries :

* Local Libraries :

.LIB "../../../lm5046-pspicefiles/lm5046.lib"

.LIB "c:/lm5xxx/lm5046example.lib"

.LIB "c:/lm5xxx/lm5046example2.lib"

* From [PSPICE NETLIST] section of C:\Users\a0967846\AppData\Roaming\SPB_Data\cdssetup\OrCAD_PSpice/16.6.0/PSpice.ini file:

.lib "nom.lib"

.stmlib "C:\LM5xxx\LM5046EXAMPLE3.lib"

.stmlib "C:\LM5xxx\LM5046EXAMPLE2.lib"

.stmlib "C:\LM5xxx\LM5046EXAMPLE.lib"

.stmlib "C:\LM5xxx\LM5046.LIB"

.stmlib "C:\Cadence\SPB_16.6\tools\pspice\library\nom.lib"

*Analysis directives:

.TRAN 0 1000ns 0

.OPTIONS ADVCONV

.PROBE64 V(alias(*)) I(alias(*))

.INC "..\Example Circuit1.net"

**** INCLUDING "Example Circuit1.net" ****

* source LM5046

C_Css SS 0 4.7n IC=0

R_Rcs3 CS2 0 10k

C_Cbst2 HS2 BST2 0.1u IC=0

D_Dbst1 VCC BST1 DNOM

D_Dbst2 VCC BST2 DNOM

C_Csssr SSSR 0 470p IC=0

C_Cres RES 0 1n IC=0

C_Cref REF 0 1u IC=0

C_Cvcc VCC 0 1u IC=0

C_Ccs CS 0 100p IC=0

R_Rt RT 0 50k

D_Dcs CS2 CS1 DNOM

R_Rdummy1 SLOPE RAMP 1m

V_Vsupply VSUPPLY 0

+PWL 0 0 0.01m 0 0.2m 36 1.2m 75 2.2m 75 2.5m 36 3m 0

R_Rwire1 VSUPPLY1 VSUPPLY2 1m

R_Rd1 RD1 0 80k

X_F_currentXfmr VSUPPLY VSUPPLY1 0 CS2 Example_Circuit1_F_currentXfmr

R_Rcs1 CS1 0 15

R_Rcs2 CS1 CS 499

R_Rd2 RD2 0 40k

R_Rdummy2 SSOFF 0 1k

R_Rramp CS RAMP 15k

R_Ruv1 VSUPPLY UVLO 100k

M_M3 VSUPPLY2 HO2 HS2 HS2 NMOSNOM

X_U5B REF_SEC FB P7V N7V COMP_SEC LM258

V_N7V 0 N7V 7

R_Rbias COMP_SEC N16934950 2k

C_Ccomp1 FB COMP_SEC 47p IC=0

C_Ccomp2 FB CP 3300p IC=0

R_Rcomp1 COMP_SEC CP 18k

V_P7V P7V 0 7

V_REF REF_SEC 0 1.2

X_U8_ext P7V N16934950 REF COMP PS2501 PARAMS: REL_CTR=1

R_Ruv2 UVLO OVP 2.6k

R_Ruv3 OVP 0 1.6k

M_M4 HS2 LO2 0 0 NMOSNOM

R_Rwire2 VSUPPLY VIN 1m

M_M1 VSUPPLY2 HO1 HS1 HS1 NMOSNOM

M_M2 HS1 LO1 0 0 NMOSNOM

C_Cbst1 HS1 BST1 0.1u IC=0

X_U6 UVLO OVP RAMP CS SLOPE COMP REF RT RD1 RD2 RES SS SSSR SSOFF HS2

+ HO2 BST2 SR2 LO2 VCC LO1 SR1 BST1 HO1 HS1 VIN LM5046

X_U7 HS1 HS2 CHB VOUT1 VOUT1 N16942154 TX1P2S PARAMS: NP=9 NS=1

L_Lpri1 HS1 HS2 240u

C_Cout1 VOUT 0 680u IC=0

L_Lout3 VOUT1 VOUT 1.6u

R_Rfbtop1 VOUT FB 25.5k

R_Rfbbot1 FB 0 15k

R_Rload1 VOUT_LOAD 0 0.11

R_Rwire9 VOUT VOUT_LOAD 1m

M_M10 CHB SR2 0 0 NMOSNOM

M_M12 N16942154 SR1 0 0 NMOSNOM

.subckt Example_Circuit1_F_currentXfmr 1 2 3 4

F_F_currentXfmr 3 4 VF_F_currentXfmr 0.01

VF_F_currentXfmr 1 2 0V

.ends Example_Circuit1_F_currentXfmr

**** RESUMING a.cir ****

.END

ERROR(ORPSIM-15108): Subcircuit TX1P2S used by X_U7 is undefined

0 Britt Brooks - Online Design Tools over 9 years ago in reply to Jerome Shin

TI__Mastermind 41310 points

Jerome,

You did not include the .lib file LM5046EXAMPLE3.lib which contains the TX1P2S model. If you add this library, PSpice should run correctly. As for the TINA-TI import, try this .lib file. There are empty PARAMS: statements that TINA-TI does not like, but PSpice ignores:

6443.lm5046.lib

The .lib files in the .zip file I provided are already corrected for this issue.

0 Jerome Shin over 9 years ago in reply to Britt Brooks - Online Design Tools

TI__Prodigy 100 points

Britt,

the lib was already added as following capture but it also showed error. (ERROR(ORPSIM-15108): Subcircuit TX1P2S used by X_U7 is undefined)

When changed the example3.lib to original one, it also can't run the simulation.

Following is the error message. Would you please let me know why the model can't run?

**** 08/25/16 18:03:58 ***** PSpice 16.6.0 (October 2012) ***** ID# 0 ********

** Profile: "Example Circuit1-a" [ c:\lm5xxx\2\lm5046-pspicefiles\example circuit1\a.sim ]

**** CIRCUIT DESCRIPTION

******************************************************************************

** Creating circuit file "a.cir"
** WARNING: THIS AUTOMATICALLY GENERATED FILE MAY BE OVERWRITTEN BY SUBSEQUENT SIMULATIONS

*Libraries:
* Profile Libraries :
* Local Libraries :
.LIB "../../../lm5046-pspicefiles/lm5046.lib"
.LIB "c:/lm5xxx/lm5046example.lib"
.LIB "c:/lm5xxx/lm5046example2.lib"
* From [PSPICE NETLIST] section of C:\Users\a0967846\AppData\Roaming\SPB_Data\cdssetup\OrCAD_PSpice/16.6.0/PSpice.ini file:
.lib "nom.lib"
.stmlib "C:\Users\a0967846\Desktop\NW\06_TI_Spec\01_HighPower_Isolated\LM5046_PSFB\LM5046_PSPICE_022511\Example\LM5046EXAMPLE3.lib""
-----------------------------------------------------------------------------------------------------------------------------------$
ERROR(ORPSIM-16377): Quoted strings must fit on one line
+ "
--$
ERROR(ORPSIM-16377): Quoted strings must fit on one line
.stmlib "C:\LM5xxx\LM5046EXAMPLE3.lib"
.stmlib "C:\LM5xxx\LM5046EXAMPLE2.lib"
.stmlib "C:\LM5xxx\LM5046EXAMPLE.lib"
.stmlib "C:\LM5xxx\LM5046.LIB"
.stmlib "C:\Cadence\SPB_16.6\tools\pspice\library\nom.lib"

*Analysis directives:
.TRAN 0 1000ns 0
.OPTIONS ADVCONV
.PROBE64 V(alias(*)) I(alias(*))
.INC "..\Example Circuit1.net"

.subckt Example_Circuit1_F_currentXfmr 1 2 3 4
F_F_currentXfmr 3 4 VF_F_currentXfmr 0.01
VF_F_currentXfmr 1 2 0V
.ends Example_Circuit1_F_currentXfmr

**** RESUMING a.cir ****
.END

0 Britt Brooks - Online Design Tools over 9 years ago in reply to Jerome Shin

TI__Mastermind 41310 points

Jerome,

You seem to be having a lot of difficulty with the PSpice symbol files and how they are set up. Please try the following .zip file that I have created for PSpice version 16.6. Unzip the files and run the opj file and it should run for you. It has been tested in 16.6 and works correctly. You should not have to change anything.

2235.LM5046_Example.zip

0 Jerome Shin over 9 years ago in reply to Britt Brooks - Online Design Tools

TI__Prodigy 100 points

Hi Britt,

Thank you very much.
I've checked your modified mode is working well.

Thanks and Best Regards.
Jerome Shin

Simulation, hardware & system design tools

Simulation, hardware & system design tools forum

How to run LM5046 PSPICE simulation model?