LTspice problem simulating LM4562, floating nodes error

Thread Starter

nidhogg_4

Joined May 9, 2016
4
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
 

Attachments

eetech00

Joined Jun 8, 2013
1,992
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?
 

eetech00

Joined Jun 8, 2013
1,992
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
 

Attachments

Thread Starter

nidhogg_4

Joined May 9, 2016
4
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
 

brianmk

Joined Dec 23, 2016
21
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.
 
Top