The simulation appears to run (I get a sensible looking gain/frequency plot).



However ltspice gives the following errors.



Any idea what the problem might be?
The .lib and .asc files are attached.

 

Hi Brian,
This is what I see if I REM out the unused Models.

E

 

Hmmm - just tried deleting the directives that include the unused op amp models.
I still get the errors.

 

Hi Brian,
I used your LM 4562 Model.
The errors in your first post relate to U1 and U2 which are the two OPA's???

E
Did you try the asc file I posted back?

BTW: Are you using Windows?

 

Just tried your asc file. I get the same errors.
If I substitute the LM4562 with any of the other op amps in the '.lib' include directives, the errors disappear.
It suggests an error in the model for the LM4562. I don't understand why you don't see the same error log.
I am using Windows 10.

 

When I get the errors, the error log pops up in a separate window.
Perhaps you need to 'View->Spice Error Log' to see the log.

 

Hi,
I did post a copy of my Spice error log.
E

 

The comments at the top of the lib file indicate the model was created for 'Pspice' rather than ltspice. Could that affect things?

** Released by: WEBENCH(R) Design Center, Texas Instruments Inc.
* Part: LM4562
* Date: 4/10/2012
* Model Type: All In One
* Simulator: Pspice
* Simulator Version: 16.2
* EVM Order Number: N/A
* EVM Users Guide: N/A
* Datasheet: SNAS326I - January 26, 2010
*
* Model Version: 1.1

 

Perhaps we have a difference in ltspice options?

 

 

 

Just tried a simplified version uisng a single op amp.
I get the same errors.

ERROR: Node U1:1:U11:VP1 is floating and connected to current source G:U1:1:U111
ERROR: Node U1:1:14 is floating and connected to current source G:U1:1:U16:R1
ERROR: Node U1:1:U11:VP2 is floating and connected to current source G:U1:1:U112
ERROR: Node U1:1:U11:VP3 is floating and connected to current source G:U1:1:U113
ERROR: Node U1:1:U11:VP4 is floating and connected to current source G:U1:1:U114
ERROR: Node U1:1:U11:VZ1 is floating and connected to current source G:U1:1:U11:Z1
ERROR: Node U1:1:U11:VZ2 is floating and connected to current source G:U1:1:U11:Z2
ERROR: Node U1:1:U11:VZ3 is floating and connected to current source G:U1:1:U11:Z3
ERROR: Node U1:1:U11:VZ4 is floating and connected to current source G:U1:1:U11:Z4
ERROR: Node U1:1:9 is floating and connected to current source G:U1:1:U11:Z5

Direct Newton iteration failed to find .op point. (Use ".option noopiter" to skip.)


As before the simulation does appear to run.

 

I am starting to think the problem may be the LM4562.asy file in the lib\sym\OpAmps folder.
The file I have is dated 2016 and may not match the LM4562.lib file.
Can you upload the one that you have?

 

Hi Brian,
Unzip this file, all my info on the device.
E

 

Your .asy & .sub files seem to have done the trick.
I renamed .sub to .lib - I don't think it makes any difference.
In my original .asy version, the 'In+' and 'In-' pins appear to be swapped relative to the .lib (or .sub) file.

I have attached my original version for comparison.
(I added a .txt extension so that I could attach it)
I can't remember where the original .asy file (dated 2016 on my PC) came from. It may have been an earlier version downloaded from the TI website or a modified version downloaded from the thread below (also dated 2016).
That thread contains a similar discussion about the model not working.

https://forum.allaboutcircuits.com/...imulating-lm4562-floating-nodes-error.123941/

It is possible that the .asy and .lib files ended up out of step. Perhaps one person corrected the mismatch by changing the .asy file while another changed the .lib file instead.

There could also have been confusion cause by library folders moving when LTspice IV changed to LTspice XV11.