I am trying to configure TI LM4562 model for the KiCad Spice simulator
using the TL072 as a template. The TL072 version is from tutorials
and they work. But the TL072 is a simple macromodel, the LM4562 is
more complex with different subckt structures.
Advice for mapping the LM4562 pins would be appreciated.
I put some “preformatted text” (triple back ticks) in your post to make the posted snippets more readable. You can find these (and more) in the “menu bar” when you’re typing a post.
I don’t think that matters. For ngSpice (The simulator in KiCad) they are just subcircuits, and complexity of their internals has nothing at all to do with pin mapping.
So far, I have found that TL072 opamp works as described in the tutorial. The LM4562 and NE/NJM-5532 are not usable. For example, pin 3 of the 5532 shows 30vdc while the power supply is ±15. The input signal is distorted. The model is from s-audio.systems
I’d like to recommend to run a simple test, if involving a new operational amplifier with a model downloaded from somewhere. This test checks if the model is compliant with KiCad/ngspice. It uses a 5-pin generic symbol and the vendor-supplied 5-pin models.
In the attached project (KiCad 9.0.3) there is a simple non-inverting amplifier with a gain of 2 and a sinewave input. The generic symbol with 5 pins is drawn from the Simulation_SPICE library. A generic model is intrinsically attached to this symbol.
As a first test you may run the op, ac, and tran simulations.
If you want to test another amplifier, do the following:
Download the model, put it into the project folder.
Attach the model to the symbol.
Take care of the pin sequence (obviously not all models have the same sequence.).
Run the simulations, check if they look similar to what obtained with the generic model. OpAmpTest.7z (6.5 KB)
The LM4562 model is different then the TL072 version. These chips have identical pins so I am surprised to see an additional subckt and I don’t understand. Perhaps I should test it as a 5pin version…
Pins 2 and 3 are swapped compared to TL072, TL082, and NE5532. Is that intentional.
According to chatGPT, LTSpice and TINA simulators silently update the 5pin models to 8pin. This means duplication of effort because everybody has to invent fixes for these incomplete models. Just saying.
Have you also asked your chatbox who and why swapped those pins?
Both me and Holger gave you pretty good hints about the problem, then your chatbox apparently suggest the same, and that is apparently still not enough to change two pin numbers.
I am pretty sure chatGPT is mistaken here. LTSpice simply uses the spice model and is usually unaware of the real physical package. E.g. the TI model for the TL072 only represents one of the op-amps inside the package. Since LTSpice doesn’t care about the real package one simply adds this op-amp model however often it is needed to the LTSpice circuit. Kicad circuits represent real devices. So the nodes in the spice model have to be matched to the pins of the real physical device.
That’s simply wrong. In reality they don’t care about the 8 pins of a real footprint. They use the 5-node model with a 5-pin symbol (pin stands for electrical node, not a real solderable pin). And if you want to simulate the two opamps in LTSPICE, you have to place 2 symbols with 5 pins each.
You cannot just use ChatGPT and be taken seriously. You must always follow up on a ChatGPT query with further research of your own to verify the answer. This is true in general, but non-trivial electronics-related LLM spew in particular should always be assumed to be of negative value until proven otherwise.
EDA tools are notoriously hard to find information on, because it’s either horribly out-of-date, undocumented, or locked away in company knowledge bases, the brains of the senior engineers and behind vendor forum login walls, which often require a subscription. In addition this lack of good information means they are frequently misunderstood and so there are very many outright wrong answers on forums that go unchallenged and just sit there for decades. There are also many discussions with just problem statements, often with mistaken assumptions and no answers or corrections. LLMs are also poor at handling things like part numbers as they tend to appear statistically linguistically interchangeable, but are very much not interchangeable in the real world.
This used to just make it hard to find information via Google. Now, it means that LLMs will also fail to find true information in their training data and via their own searching, also ingest a lot of wrong information and then they’ll often make something plausible-sounding up.
Now, ChatGPT may indeed be able to magic up a good answer and give you the keywords and even links to go and verify it. In fact it’s extremely good at it, and using it is a fine idea. But you have to then do the verification bit. Every time, personally, and before you dump the quantum answer-hallicination superposition on forums for others to verify or debunk for you.
As for the pin mapping, it’s very normal that the model doesn’t have the same signal ordering as the physical components. In fact it’s pretty unusual for it to match, and also usual that it nearly matches. You have to remap the signal here to match the model to the pins on the KiCad symbol
If you are having convergence problems, you might add 10 megohm or feedback around the op amp so dc settles better. You could also temporarily try connecting R4 to the opamp output instead of the FB node to see if that works first.
* file: LM4562_8pin.lib
*
* align KiCad 8pins to the vendor's 5pin SPICE model
* 2025.08.02
.subckt LM4562_8pin 1out 1in- 1in+ vcc- 2in+ 2in- 2out vcc+
.include LM4562_5pin.lib ; VDD VSS VIP VIM VO
XU1A
+ vcc+ ; VDD in LM4562_5pin
+ vcc- ; VSS
+ 1in+ ; VIP
+ 1in- ; VIM
+ 1out ; VO
+ LM4562_5pin
XU1B vcc+ vcc- 2in+ 2in- 2out LM4562_5pin
.ends LM4562_8pin
I think KiCad uses the real dual opamp bins to decide the order of the virtual pins. If one uses XU1 to match the model pins, then the pin ordering tool in the simulation editor is not needed.
Another concern is that the vendor’s LM4562 has an extra subckt to reorder the incoming parameters a second time. Perhaps this is just to match some unknown simulator. I find this confusing and unnecessary so I deleted subckt LM4562 and and renamed subckt AMP to LM4562_5pin.
I added file LM4562_8pin for dual opamp operation.
* file: LM4562_5pin (snippet)
* These parameters must be aligned in LM4562_8pin.lib
*
.SUBCKT LM4562_5pin VDD VSS VIP VIM VO
Iq VDD VSS 5E-3
IS2 VDD 6 -15.5E-9
IS3 5 VSS 4.5E-9
I attach a simple KiCad project if you want to experiment. K3.zip (13.8 KB)
My previous post explained how to expand the LM4562 model from 5pin to 8pin as it ought to be. However it was based on the tutorial which requires two files. Nothing wrong with but I believe the task can done with just one file. It requires a simple change to the official LM4632 model file.
First find the AMP subckt and delete any subckts above. Next insert the following:
.subckt LM4562_8p 1out 1in- 1in+ vcc- 2in+ 2in- 2out vcc+
XU1A
+ vcc+ ; VDD in LM4562_5pin
+ vcc- ; VSS
+ 1in+ ; VIP
+ 1in- ; VIM
+ 1out ; VO
+ AMP ; side A instance
XU1B vcc+ vcc- 2in+ 2in- 2out AMP ; side B instance
.ends LM4562_8p
*$
KiCad automatically assigns the correct symbol-to-model pins as shown int the Simulation Editor snapshot.
