2
\$\begingroup\$

I'm new to LTSpice but have the basics figured out (laying out a schematic, setting up simulation, running) and have done so with the basic but very well stocked library included. Of course my issue is I'm not using LT op amps.

I'm trying to import the model for the LM4562, but there are three options: PSPICE, and two TINA-TI which I'm not even sure what that is. The PSPICE package does not contain any .mod or .subckt files, rather it contains a .lib that has all the subcircuit information in it.

I have been trying for the last few hours to import the parameters and get it to work to no avail. All the tutorials are usually directed either at .mod files, or when I try to .INCLUDE the .LIB file, it throws errors that I don't fully understand.

I used the opamp2 symbol and modified it so that the pin names match up, or at least I believe I did (I could have done it incorrectly I suppose).

Below is a screenshot of the circuit I'm using to test it, and the error message I get:

enter image description here

Below is my Netlist:

D:\Projects\Electronics!TestCCt\opamp test.asc

V1 VCC 0 9

V2 0 VEE 9

V3 Vni 0 SINE(0 1 500)

R1 0 Vi 1K

R2 OP Vi 9.09K

XU1 Vi Vni VCC VEE OP LM4562

.INCLUDE D:\Library\Datasheets\Models\lm4562\LM4562.LIB

;op

.tran 0 25ms 0s 1ms

.backanno

.end

Errors are as follows. I'm not sure what nodes are floating:

**Circuit: * D:\Projects\Electronics!TestCCt\opamp test.asc

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. (Use ".option noopiter" to skip.) Starting Gmin stepping Gmin = 10 Gmin = 1.07374 vernier = 0.5 vernier = 0.25 vernier = 0.125 Gmin = 1.02385 vernier = 0.0625 vernier = 0.03125 vernier = 0.015625 Gmin = 1.01955 vernier = 0.0078125 vernier = 0.00390625 Gmin = 1.0126 vernier = 0.00520833 vernier = 0.00260417 vernier = 0.00130208 Gmin = 1.00833 vernier = 0.000651042 vernier = 0.000868055 Gmin = 1.00696 vernier = 0.00115741 vernier = 0.000578703 Gmin = 1.00536 vernier = 0.000771604 vernier = 0.000578703 vernier = 0.000771604 vernier = 0.000578703 Gmin = 1.00449 vernier = 0.000434027 vernier = 0.000578703 Gmin = 1.00351 vernier = 0.000434027 Gmin = 0 Gmin stepping failed

Starting source stepping with srcstepmethod=0 Singular matrix: Check node u1:1:u11:vz3 Iteration No. 1 Singular matrix: Check node u1:1:9 Iteration No. 2 Could not converge to DC with sources off! Starting source stepping with srcstepmethod=1 Singular matrix: Check nodes u1:1:14 and u1:1:9 Iteration No. 1 Could not converge to DC with sources off! Singular matrix: Check node u1:1:9 Iteration No. 1 Fatal Error: Singular matrix: check node u1:1:9 Iteration No. 1

This circuit has floating nodes.**

What am I doing wrong, and more importantly, how do I import this model correctly?

\$\endgroup\$
0

2 Answers 2

Reset to default
2
\$\begingroup\$

It looks like the op amp symbol you dropped in your schematic is not mapping to the correct pins on the device. What symbol did you use? You can make a new symbol and make sure the pin names match those in the .lib file...

\$\endgroup\$
10
  • \$\begingroup\$ Thank you. I did exactly that, as well, modifying "opamp2" and saving it as a customized symbol "TIopamp" - this is actually all taken from after I assured the pin names were the same. If I can take a screenshot or provide any other information please let me know. I've also included this information in an edit in the above post for reference \$\endgroup\$
    – MJXS
    Jul 23, 2014 at 16:41
  • \$\begingroup\$ Can you attach your netlist? (View->SPICE netlist) \$\endgroup\$
    – user49628
    Jul 23, 2014 at 16:42
  • \$\begingroup\$ I will try, one moment There we are, see above \$\endgroup\$
    – MJXS
    Jul 23, 2014 at 16:42
  • \$\begingroup\$ I see a few problems. If you look at the order of the pins in the netlist it does not match the order in the .lib file. Secondly, you have a negative voltage on your positive supply rail. Also, you have a positive voltage on your negative rail! \$\endgroup\$
    – user49628
    Jul 23, 2014 at 16:53
  • 1
    \$\begingroup\$ Notice that the signal inputs are still before the supply nets in the netlist. It believe it should be XU1 VCC VEE Vi Vni OP LM4562... It seems that LTSPICE is not mapping the pins correctly from your symbol. You can either fix this manually and run from the netlist or you can try to get to the bottom of it. It might work if you start a symbol from scratch instead of editing and old one? Just a guess... \$\endgroup\$
    – user49628
    Jul 23, 2014 at 17:34
0
\$\begingroup\$

There are two ways: The first is: Click on the ".OP" button, type .lib and insert it in Schematic, then with the right mouse button click on the created directive and go look for the LIB file (spicemodel) you want to implement, in the location where you saved it. Open Spice Model and look for the correct name of the document and insert a generic component, but of the same nature as yours, for example an NPN Transistor, then right-click on the generic component and change its name by the component name that is written in the Spice Model. Ready. The second alternative is: Open the Spice model with Ltspice, right-click on the Spice model's name, a list will appear, click on the "Creating Simbol" option, it will be in the Auto-Generated components folder in Ltspice, and there's still how to modify the created Symbol Layout if you want. Then just use it normally without having to use the ".inc" and ".lib" directives.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge that you have read and understand our privacy policy and code of conduct.

Not the answer you're looking for? Browse other questions tagged or ask your own question.