TPS7H5001-SP: Unable to sim transient model in PSpice for TI

Hey Andre,

What simulation software are you using when running this simulation?

Thanks,

Daniel

Hi Daniel, I'm using PSpice for TI 17.4-2021 S007

Hey Andre,

I was able to confirm your issue on my end.
I believe this is either an issue of us giving incomplete files or with the model.

I will continue to investigate this and give updates as I go.

Thanks,

Daniel

A Good that some others have also the same Problem :) Hope they update the model as soon as possible, that i can go on with my tests with this chip. I use TINA. 9.3

Hey Josef,

Are you seeing the exact same issue or a similar one?

Thanks,

Daniel

Hey Josef/Andre,

I have confirmed this is a common issue between free PSPICE simulators that is not common with the paid versions.
I am still investigating if there is a solution available.

Thanks,
Daniel

Hi Daniel,

I get the same Problem with the VCO_SQR as Andre gets.

"Undefined subcircuit: VCO_SQR. (C:\Program Files (x86)\DesignSoft\Tina 9 - TI\EXAMPLES\SPICE\TSPICE.LIB)

But i get only the VCO_SQR displayed. Tina stop, as i see, at the first error and does not check the rest.
That could also be fixed in Tina, to get all the problems in one punch instead of going one after the other .

Regards
Josef

Thank you for the information Josef.

Daniel

Hey Daniel,

thx for the info. That info should be added at the spice model download, or in the spice file as comment,
that the people know that in advance :).
As long this is not resolved, can you give me a link where i can get this library?

Regards
Josef

If you are using the model in LTSpice you can include the following statements as Spice Directives in the schematic and it seems to allow the model to function.

.subckt vco_sqr in out Params: Fcenter=2e6 Frange=2e6 Vmin=0 Vmax=4MEG
+phase=0
 
 
Rin             in              0               1G
Rtable  table   0               1G
 
Etable  table   0       Value {Table(V(in),Vmin,-1,Vmax,1)}
 
Esin            sine            0               
+Value {sin(6.28318*(Fcenter*time+Frange*SDT(V(table)))+phase*(3.14159/180))}
 
Esqr            out             0               table {V(sine)} (0,0) (1n,1)
 
.ends
 

.SUBCKT AWBONE_SHOT 1 11 8 PARAMS: DELAY= 1U
.PARAM CC={0.002*DELAY}
SS10 9 0 8 0 MS1MSS10
.MODEL MS1MSS10 VSWITCH VT=499.999970M VH=1N RON=1G ROFF=1M
II8 0 9 1.000000M
CC1 9 0 {CC}
SS9 5 4 11 0 MS2MSS9
.MODEL MS2MSS9 VSWITCH VT=499.999970M VH=1N RON=1 ROFF=1MEG
SS8 5 4 9 0 MS2MSS9
II7 0 4 -2U
VV3 5 0 1
II6 0 2 2U
SS7 0 2 4 0 MS2MSS9
SS6 0 2 1 0 MS2MSS9
II5 0 7 1U
SS5 0 7 4 2 MS3MSS5
.MODEL MS3MSS5 VSWITCH VT=0 VH=499.999970M RON=1 ROFF=1MEG
GV2 0 6 7 0 2U
SS4 6 0 2 0 MS4MSS4
.MODEL MS4MSS4 VSWITCH VT=499.999970M VH=1.000000N RON=1K ROFF=1MEG
II4 6 0 1U
II3 0 8 1U
SS3 8 0 6 0 MS5MSS3
.MODEL MS5MSS3 VSWITCH VT=0 VH=499.999970M RON=1MEG ROFF=1
GV1 0 3 0 0 -2U
SS1 3 0 1 0 MS4MSS4
II1 3 0 -1U
II2 0 7 1U
SS2 7 0 3 0 MS5MSS3
.ENDS AWBONE_SHOT

Hey Thomas,

I can confirm that is actually what we are trying to implement into the model now and get it released.

The problem specific to PSPICE for TI is that there is a limit on the number of traces probed.
TINA may not have an issue, but this is certainly a fix for LTSPICE.

I will update the forum here when we get through the release process.

Thanks,

Daniel