importing opamp component problem

[yefj]

Hello,I have a opamp component shown in the link bellow.
I have created a simbol from the netlist and constructed a basic circuit to use the opamp as a comparator.
But it shows me these errors.
Where did i go wrong?
Thanks.

https://www.maximintegrated.com/content/dam/files/design/tools/modeling-simulation/spice/analog/amplifiers/operational-amplifiers/MAX4231.lib

.SUBCKT MAX4231 1 2 3 4 5 6
*               | | | | | |
*               | | | | | nSD
*               | | | | Output
*               | | | Negative Supply
*               | | Positive Supply
*               | Inverting Input
*               Non-inverting Input
*

 

[KlausST]

Hi,

Sorry, I can't help you with your problem.

But please use standard schematic symbols.
A black box with numbers 1...6 is not a useful symbol. Nobody knows what it means.

Standard symbols really make sense.

Klaus

 

[stenzer]

Hi,

But please use standard schematic symbols.

this is the standard symbol which is generated by default in LTspice when importing/creating a component in LTspice. Unfortunately, the creation/drawing of a "new" symbol is not that intuitive (one has to know the hot-keys).

Pin 6 seems to be active low (nSD), aslo according to the datsaheet, so please run your simulation again while enabling the IC, by maens of applying VDD to pin 6.

BR

 

[crutschow]

The way I import an op amp model into LTspice is to edit the .asy symbol file of an op amp with the same number of pins, and just change the pin designations and model reference to the new op amp.
Then save it as a new .asy file.

Below is a sample edit for the LM324.asy op amp file.
You right click on each pin to establish the Netlist Order as shown in the .subckt file.
Do you do that so all the pins (squares) in your .asy file match the numbers on your symbol?

 

[dick_freebird]

Two floating nodes with current sources could be causing
a "blowup". You should inspect the op amp netlist and
those nodes' voltages (if your simulator will give a value
despite failing to converge) and figure out whether this
is the problem, or just a complaint.

You should also look at the Maxim model regarding what
simulator it purports to work with. Behavioral models are
an industry norm, but different simulators support different
behavioral languages and LTSpice is extra-special-different.
A (say) PSpice macromodel might need some massaging
to play right in LTSpice and vice versa.

Might also check that "units" complaint and make sure
you are not having a simulator default units problem
(like MKS and cgs, what you call "1u" could be a micron
gate L in a MKS-default simulator and a 10nm L in one
that uses cgs as default.

 

[FvM]

It's no import issue, the model is connected correctly in post #1, except for disabling the OP by grounding nSD pin. Model comment says

Use PSPICE (or SPICE 2G6; other simulators may require translation)

MOSFET size warning messages indicate a model incompatibility. If you need to run this model in LTspice, you can try to get help at support forum https://groups.io/g/LTspice