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

The simulator is still complaining, now about a singular matrix.  Could you provide the complete updated model?  Maybe I am not placing these added resistors in the right place in the subcircuits.  I have added R1000, R2000, and R3000.

Hello,

  Thanks for trying it out. I have attached the .lib file in the last reply, does that file work for you?

Thank you,
Sima

No it did not work.  

Interestingly, when I change the supply voltage to 5V, it works. But the part is only rated to 3.3V.

Hello,

   Thanks for the update. The OPA858 is rated up to 5.25 recommend max voltage, while OPA857 is rated up to 3.6 recommend max voltage. The OPA858 should still work at 3.3V. It might be either the conversion to a different simulator than the ones we recommend (Tina-TI or PSpice for TI) or violating at input/output specification of the device since it is different compared to OPA857.

Best Regards,
Sima