OPA857: OPA857 Spice Model

Hello,

  Yes, this is a known error when importing this netlist into LTSpice. The reason this occurs is because the current source used to create the model needs a DC connection to ground which LTSpice does not automatically add. We can fix this error by adding a very large resistance to ground to provide the simulation a DC path to ground for compilation.

  Here are two threads that had the same issue, and was fixed by adjusting the netlist: 

1. https://e2e.ti.com/support/amplifiers-group/amplifiers/f/amplifiers-forum/1371174/opa695-opa695-pspice-file-seems-broken#
2. https://e2e.ti.com/support/amplifiers-group/amplifiers/f/amplifiers-forum/1060033/opa835-error-in-spice-model#

  Therefore OPA857 netlist needs to be adjusted to add the two lines in red: 

EA 101 GNDF 1 GNDF 1
GRA 101 102 VALUE = { V(101,102)/1e6 }
CA 102 GNDF 1e3
EB 1 1a VALUE = {V(102,GNDF)}

R1000 102 0 10MEG

E1 VO VI 1a GNDF 1
C2 VDD VSS 10P
.ENDS

G2 GNDF 3 VSS GNDF {GPSRRN}
R2 3 4 {RPSRRN}
L2 4 GNDF {LPSRRN}

EC 301 GNDF 3 GNDF 1
GRC 301 302 VALUE = { V(301,302)/1e6 }
CC 302 GNDF 1e3
ED 3 3a VALUE = {V(302,GNDF)}

R2000 302 0 10MEG

E1 VO VI VALUE = {V(1a,GNDF) + V(3a,GNDF)}
C3 VDD VSS 10P
.ENDS

Thank you,
Sima 

Hello Sima, I tried adding those lines but I still get the error message:

ERROR: Node U2:I0:I5:I19:1:102 is floating and connected to current source G:U2:I0:I5:I19:1:RA

u2:i0:i5:v0: Missing value, assumed 0V @ DC
u2:i0:i5:v1: Missing value, assumed 0V @ DC
Per .tran options, skipping operating point for transient analysis.
Ignoring empty pin current: Ix(u2:ctrl)
Changing Tseed to 9.76563e-011

Hello,

  It looks like there is another 102 node in the lib file: I added another line:

R3000 102 0 10MEG

  Attached below is the edited .lib file:

opa857.lib

Thank you,
Sima

Hello,

this seems to have resolved the issue.  But there is a similar problem with the OPA858.  In fact, most of the TIA models seems to have the same issue.  Can you look at the one for OPA858:

ERROR: Node U1:I0:I21:1:102 is floating and connected to current source G:U1:I0:I21:1:RA
ERROR: Node U1:I0:I19:1:102 is floating and connected to current source G:U1:I0:I19:1:RA
ERROR: Node U1:I0:I19:1:302 is floating and connected to current source G:U1:I0:I19:1:RC

u1:i0:vprobe1: Missing value, assumed 0V @ DC
u1:i0:vprobe2: Missing value, assumed 0V @ DC
Direct Newton iteration for .op point succeeded.

Hello,

  I am glad that fixed the issue. Yes, this is a common issue with converting to LTSpice. We recommend using Tina-TI or PSpice for TI for our sim models.

  To fix the OPA858 netlist, you would include the same lines:

R1000 102 0 10MEG
R2000 102 0 10MEG
R3000 302 0 10MEG

  Attached is the adjusted netlist.

2553.OPA858.LIB

Thank you,
Sima