• Welcome to our site! Electro Tech is an online community (with over 170,000 members) who enjoy talking about and building electronic circuits, projects and gadgets. To participate you need to register. Registration is free. Click here to register now.

Really basic LTSpice question

Thread starter #1
I use some simple SPICE simulations as part of an electronics course I teach. In the past, I've had students download ngspice, but I was going to try LTSpice this year, because it's more user friendly. Unfortunately, I can't seem to make it work on even the simplest of our examples. For example, the transient analysis below returns "Run: missing node(s)". I've run this on just about every version of SPICE and it works fine.

Any advice would be appreciated.

Thanks in advance.


EXAMPLE 3 LRC
***Begin netlist
R1 1 2 100
C1 1 0 1mF
L1 2 0 100
***End netlist
***Specify initial condition (5V at node 1) with .IC command
.IC V(1) = 5
***Perform transient analysis
.TRAN 0.1s 20s
***Begin control block
.control
run
plot V(1) V(2)
.endcontrol
***End control block
.end
 

crutschow

Well-Known Member
Most Helpful Member
#3
I haven't worked from a Spice netlist in at least 20 years, and if you are still using netlists in your electronics course you are well behind the state-of -the art (unless you are using it just to demonstrate how Spice internally describes a circuit) .
So below is the LTspice simulation from the generated schematic with its attached .asc file.
The netlist generated from the schematic is below the schematic.

1539662425764.png
1539664128575.png
 

Attachments

Last edited:

alec_t

Well-Known Member
Most Helpful Member
#4
Has the sim text been entered on a schematic as a command or as a comment?
 

eTech

Active Member
#5
I use some simple SPICE simulations as part of an electronics course I teach. In the past, I've had students download ngspice, but I was going to try LTSpice this year, because it's more user friendly. Unfortunately, I can't seem to make it work on even the simplest of our examples. For example, the transient analysis below returns "Run: missing node(s)". I've run this on just about every version of SPICE and it works fine.

Any advice would be appreciated.

Thanks in advance.


EXAMPLE 3 LRC
***Begin netlist
R1 1 2 100
C1 1 0 1mF
L1 2 0 100
***End netlist
***Specify initial condition (5V at node 1) with .IC command
.IC V(1) = 5
***Perform transient analysis
.TRAN 0.1s 20s
***Begin control block
.control
run
plot V(1) V(2)
.endcontrol
***End control block
.end
Hi

If you've used many versions of spice, you would know that all spice's are not created equal.:)

The "Run:missing node(s)" message is due to LTspice's interpretation of the unsupported statement "run" as having no connecting nodes. :cool:
Its interpreting "run" using its leading "r" as a resistor with no connecting nodes.:)

While LTspice is somewhat PSpice compatible, LTspice does not support .control, .endcontrol, plot and run statements, so you will need to comment those out.

See below.
********
R1 1 2 100
C1 1 0 1mF
L1 2 0 100
***End netlist
***Specify initial condition (5V at node 1) with .IC command
.IC V(1) = 5
***Perform transient analysis
.TRAN 0.1s 20s
***Begin control block
*.control
*run
*.plot V(1) V(2)
*.endcontrol
***End control block
.end
********
eT
 
Last edited:

crutschow

Well-Known Member
Most Helpful Member
#6
Adding to eTech's comments, I think LTspice can only be run using the "Run" 1539705982748.png command in the LTspice window.
 

dr pepper

Well-Known Member
Most Helpful Member
#7
Its a way back so I dont quite remember, however I had issues getting ltspice to run in win7, it worked on my old xp machine, but not w7, I think it was something in the component library, schematics loaded but wouldnt sim.
 

Latest threads

EE World Online Articles

Loading

 
Top