Hi, I have been trying to simulate a simple transimpedance amplifier using the current feedback opamp LM4562 but I am getting this errors when I run the simulation:

WARNING: Node U1:1:U11:VP1 is floating.
WARNING: Node U1:1:14 is floating.
WARNING: Node U1:1:U11:VP2 is floating.
WARNING: Node U1:1:U11:VP3 is floating.
WARNING: Node U1:1:U11:VP4 is floating.
WARNING: Node U1:1:U11:VZ1 is floating.
WARNING: Node U1:1:U11:VZ2 is floating.
WARNING: Node U1:1:U11:VZ3 is floating.
WARNING: Node U1:1:U11:VZ4 is floating.
WARNING: Node U1:1:9 is floating.

Direct Newton iteration failed to find .op point.
Singular matrix: Check nodes u1:1:u11:vz2 and u1:1:u11:vz1
Iteration No. 1
Fatal Error: Singular matrix: check nodes u1:1:u11:vz2 and u1:1:u11:vz1
Iteration No. 1

This circuit has floating nodes.

The circuit I am using is attached.

Any ideas of how could I solve this? I looked into the model file but I don't understand it too well.

Thank you

 

Hi, I have been trying to simulate a simple transimpedance amplifier using the current feedback opamp LM4562 but I am getting this errors when I run the simulation:

WARNING: Node U1:1:U11:VP1 is floating.
WARNING: Node U1:1:14 is floating.
WARNING: Node U1:1:U11:VP2 is floating.
WARNING: Node U1:1:U11:VP3 is floating.
WARNING: Node U1:1:U11:VP4 is floating.
WARNING: Node U1:1:U11:VZ1 is floating.
WARNING: Node U1:1:U11:VZ2 is floating.
WARNING: Node U1:1:U11:VZ3 is floating.
WARNING: Node U1:1:U11:VZ4 is floating.
WARNING: Node U1:1:9 is floating.

Direct Newton iteration failed to find .op point.
Singular matrix: Check nodes u1:1:u11:vz2 and u1:1:u11:vz1
Iteration No. 1
Fatal Error: Singular matrix: check nodes u1:1:u11:vz2 and u1:1:u11:vz1
Iteration No. 1

This circuit has floating nodes.

The circuit I am using is attached.

Any ideas of how could I solve this? I looked into the model file but I don't understand it too well.

Thank you

You need to specify a model file defining the opamp. Did you check the TI website?

 

You need to specify a model file defining the opamp. Did you check the TI website?

I do have the model file and I did specified it by using .lib command. The model file I am using is attached to this response.

 

Post your LTspice .asc file please.

 

Post your LTspice .asc file please.

Attached asc file. Thank you for the help!!!

 

Hi

I've attached a zip file with a "fixed" LM4562Fixed.LIB" file
It should work now.

Schematic changes:
I used an unmodified built-in LTspice opamp2 symbol.
I included the LM4562Fixed.LIB file.

LM4562.LIB file changes:
was:
.SUBCKT LM4562 Vinm Vinp VCC VEE Vout
changed to:
.SUBCKT LM4562 Vinp Vinm VCC VEE Vout

was:
EGNDF GNDF 0 VALUE = {(V(VDD)+V(VSS))*0.5} <--this resolves to "0"
changed to:
EGNDF GNDF 0 VALUE = {V(VDD,VSS)*0.5}

You should let TI know there is an error in the LM4562.LIB spice file

 

Hi

I've attached a zip file with a "fixed" LM4562Fixed.LIB" file
It should work now.

Schematic changes:
I used an unmodified built-in LTspice opamp2 symbol.
I included the LM4562Fixed.LIB file.

LM4562.LIB file changes:
was:
.SUBCKT LM4562 Vinm Vinp VCC VEE Vout
changed to:
.SUBCKT LM4562 Vinp Vinm VCC VEE Vout

was:
EGNDF GNDF 0 VALUE = {(V(VDD)+V(VSS))*0.5} <--this resolves to "0"
changed to:
EGNDF GNDF 0 VALUE = {V(VDD,VSS)*0.5}

You should let TI know there is an error in the LM4562.LIB spice file

Thank you so much for the help!!!!! It works

 

OK, this is an old thread, but I am having the same problem, even when I use the "fixed" version of the Texas Instruments SPICE model for the LM4562.

After trying several different things, using a simple inverting amplifier test simulation, the one thing that made a difference was to specify a source resistance of something other than zero for the voltage sources used for Vcc and Vee. Values of 0.1 Ohms for my test simulation seem to work. A value of 0 gives the floating nodes error - both when trying transient and ac analysis.

When I use the model in place of a TL072 in a fully blown simulation of a wien bridge oscillator, I get the floating nodes error irrespective of the values used for the supply source resistance.

If I use the National Semiconductor spice model for the LME49860 (which I believe is identical to the LM4562), then things work as expected.

I think there is something not quite right with the TI model but I don't have the SPICE expertise to fix it.
Has anyone else found this problem? is there a fix?

I can upload the simulation files if anyone is interested in trying it.