LM4562

[greenm01]

Has anyone successfully gotten the TI spice model for the LM4562 to work in LTSpice? I tried importing the model myself, but I'm having issues getting everything setup properly.... Any help would be appreciated.

 

[esgigt]

What you need is an .asy model working together with your model-file.
You can make this file from scratch, but you can also copy the .asy model of an other opamp (with same connections) and rename it.

In the model-file, the part ought to be defined as a .SUBCKT for this to work. Check that the connectors in the .SUBCKT model check-out with the connections in the .asy model!!! If it doesn't, it will not work.

The model file ( with a .lib, .sub or .txt extension ) ought to be stored in the C:\Program Files (x86)\LTC\LTspiceIV\lib\sub directory

and the .asy file in the C:\Program Files (x86)\LTC\LTspiceIV\lib\sym directory.

But that's not all.

In the .asy file you've got to verify that the attribute "modelfile" has the same name as the model-file.

 

[sbrads]

You can always auto generate a symbol direct from the model.
File>Open and load in the model to show the listing.
Place the cursor on the 1st line, i.e. the line with the device name in, and right click on it & select Create Symbol.
This will be a box shape with all the correct component pins and it will reside in the Auto Generated folder when you choose a component for your schematic.

 

[udok]

The LM4562 model has some convergence problems due to an "ideal" diode. Additionally the + and - input are exchanged.
I have included the corrected file.

To add the LM4562 in your simulation add the symbol Opamps/opamp2 and rename it to LM4562. Additionally add ".lib LM4562.lib" to your circuit.

Greetings,
Udo

 

[DPH]

Realize this is a slight thread necro, but:

Udo--I was having convergence problems galore and trying to figure out what was wrong. Just found your post and wanted to thank you for your updated/corrected file.

 

[jeanbaptiste]

Thanks Udo for the updated model.

 

[brianmk]

I am also having problems with the spice model for the LM4562.

I am using the corrected version posted in this thread.
If I simulate a simple inverting amplifier test circuit using the model, it works fine.

However, if I substitute a TL072 with the LM4562 in a simulation of a 1kHz audio oscillator circuit, I get floating node and singular matrix error messages:-

===
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.

WARNING: Less than two connections to node OUT. This node is used by R12.
Early termination of direct N-R iteration.
Direct Newton iteration failed to find .op point. (Use ".option noopiter" to skip.)
Starting Gmin stepping
Gmin = 10
vernier = 0.5
vernier = 0.25
vernier = 0.125
Gmin = 5.5165
vernier = 0.0625
vernier = 0.03125
vernier = 0.015625
vernier = 0.0078125
Gmin = 5.48432
vernier = 0.00390625
vernier = 0.00195313
vernier = 0.000976563
vernier = 0.000488281
Gmin = 0
Gmin stepping failed

Starting source stepping with srcstepmethod=0
Singular matrix: Check node u1:1:u11:vz4
Iteration No. 1
Singular matrix: Check nodes u1:1:u11:vz2 and u1:1:u11:vz3
Iteration No. 1
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 nodes u1:1:9 and u1:1:u11:vz1
Iteration No. 1
Fatal Error: Singular matrix: check nodes u1:1:9 and u1:1:u11:vz1
Iteration No. 1

This circuit has floating nodes.
===

Can any LTSpice gurus suggest what might be going wrong?

I have attached a zip file containing the Oscillator3.asc file along with simulation models for the TL072 and LM4562.

 

[diyralf]

subscribed

 

[Monte McGuire]

Not sure if this is still an issue, but the LME49710 model seems to work properly, and the LME49710 is the identical single amplifier to the LM4562. I use the LME49710 model for my circuits that use the LME49720 or LM4562 and everything seems to work as expected.

The link doesn't seem to be working now, I guess because someone "cleaned up" the web site and removed links to the end of life LME49710. The silly thing is that the dual LME49720 still has Active product status, yet there is no link to a model for the LME49720, which could be a link to the LME49710.

So, pardon me TI for re-posting this, but attached is a copy of the LME49710 model from TI that I've been using successfully. If anyone at TI is annoyed by this, just attach your LME49710 PSPICE model to the LME49720 Software / Tools page and people will be happy again. For everyone out there, just change the extension from .txt to .lib as you would normally, and enjoy.

It is a truly fine amplifier, and the model seems to work very accurately, at least regarding dynamics - no reason for it to be lost.

 

[diyralf]

I am using this model too. But the LM4562 model looks very different?

 

[carlmart]

Which is you LM4562 model? Is for LTSpice?

I think mine has something wrong.

 

[Monte McGuire]

The LME49710 model seems to work well, but that went away because that chip is end-of-life. I've zipped it up and attached it here - sorry TI, but it's awfully rude to trash perfectly useful documentation, especially when there's no LME49720 model and the LM4562 model might be broken.

Hope it works for you!

 

[diyralf]

The LM4562 is not eol. Where did you read that? TI wanted to fire him a few years ago because the fab was relocated. But he continues to produce because the LME series is the best and very successful in sales. N.B. LME49710=LME49870; LM4562=LME49720=LME49860, LME49740(quad).

 

[carlmart]

So which is the LM4562 model to use that has any meaning?

 

[Monte McGuire]

As I stated, the LME49710 is EOL, not the LM4562, and that's why the LME49710 SPICE model is no longer available from TI. The LM4562 is not EOL but the model has problems. The LME49710 is basically the same amplifier as the LM4562, so the LME49710 model is appropriate to use for the LME49720, which has no SPICE model, or the LM4562, which has a flawed model.

carlmart: use the LME49710 model. I forgot that I already posted this earlier in the thread. Nothing has changed since then - use the LME49710 model for the LM4562.

 

[carlmart]

Can you please load the file I can use here and how to add it to LTSpice?

 

[dotneck335]

I still can't get a working LM4562 model for LTspice XVII. I tried the above LME49710.lib file and it don't do anything. All the other opamp models are .asy files, not .lib. I tried renaming the LME49710.lib to LME49710.asy, but that didn't work either. What am I doing wrong?

 

[jan.didden]

A .asy is just the symbol on the schematic. It has to be linked to a model which is a .lib or a .cir. So you need both.
If you right-click the symbol you see what LTspice thinks it points to and where it is.
The other thing is that the pinout on the .asy must be the same order as for the model.

There is a thread here about his.

Jan

 

[Monte McGuire]

Put the .lib file in a directory where it can stay around without causing problems (i.e. not a temp or downloads directory). Open the .lib file using LTspice. Scroll down to the .subckt line which will be highlighted in a different color, right click on the .subckt name and a menu pops up which will allow you to create a symbol for this subcircuit. A generic rectangular box will appear, and you can rename the ports from 1, 2, 3 etc. to something useful like in+, in-, V+ etc. Save, close, and now you have a model stored in your AutoGenerated models folder.

I am writing this from memory and the Mac and PC versions may be slightly different but this is the basic procedure you want to use. Here's an official piece of documentation on how to do it: LTspice: Simple Steps to Import Third-Party Models | Analog Devices

 

[diyralf]

I still can't get a working LM4562 model for LTspice XVII. I tried the above LME49710.lib file and it don't do anything. All the other opamp models are .asy files, not .lib. I tried renaming the LME49710.lib to LME49710.asy, but that didn't work either. What am I doing wrong?

Run this and have a good life. No problems at all. ltspice is not very good in lib management.