Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

importing opamp component problem

yefj

Advanced Member level 2
Joined
Sep 12, 2019
Messages
521
Helped
0
Reputation
0
Reaction score
2
Trophy points
18
Activity points
2,795
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.

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

1620423770705.png

1620423825813.png

1620424382214.png
 

KlausST

Super Moderator
Staff member
Joined
Apr 17, 2014
Messages
19,928
Helped
4,368
Reputation
8,745
Reaction score
4,347
Trophy points
1,393
Activity points
131,909
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

Advanced Member level 2
Joined
Oct 1, 2012
Messages
516
Helped
96
Reputation
192
Reaction score
112
Trophy points
1,323
Activity points
5,661
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

Advanced Member level 5
Joined
Feb 22, 2012
Messages
3,876
Helped
922
Reputation
1,842
Reaction score
909
Trophy points
1,393
Location
Colorado USA Zulu -7
Activity points
21,904
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?

1620431075515.png
 

dick_freebird

Advanced Member level 5
Joined
Mar 4, 2008
Messages
7,343
Helped
2,135
Reputation
4,275
Reaction score
2,000
Trophy points
1,393
Location
USA
Activity points
58,844
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

Super Moderator
Staff member
Joined
Jan 22, 2008
Messages
48,515
Helped
14,271
Reputation
28,805
Reaction score
12,974
Trophy points
1,393
Location
Bochum, Germany
Activity points
280,590
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
 

LaTeX Commands Quick-Menu:

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top