Setting LT Spice Simulation Time

Thread Starter

brightnight1

Joined Jan 13, 2018
75
I must be doing something wrong because my LT spice DC transient analysis is taking forever to run a simple simulation. I set it to run from 0 to 500ms:

Time_stamp_spice_2.JPG




However, after it's been running for a while I look at the time stamp in the bottom left corner and it appears to be ready a time that's much greater then 500ms. In this example it says 52.0094s. When I hit escape it stops running and seems to stop drawing the simulation results. What am I dong wrong or is the time in the bottom left hand corner just the simulation run time?

Time_stamp_Spice_1.JPG
 

Papabravo

Joined Feb 24, 2006
16,165
The simulation may seem simple to you, but I assure you there is a great deal going on under the hood that takes real time to compute. This is especially true with oscillators and rapidly changing signals with rapidly changing derivatives. The presence of a pseudo-transient analysis is indicative of difficulty in establishing a DC operating point.
 

crutschow

Joined Mar 14, 2008
27,232
The simulation time depends greatly on the circuit you are simulating.
The higher the frequency of the signals in the circuit, the longer it will take to run a specified simulation time.
Normally you want to run the minimum number of cycles of the highest frequency present that will show the circuit steady-state operation.
What exactly is your "simple simulation" of?

And why did you specify the maximum timestep, which can increase the simulation time?
Normally Spice will select the optimum timestep for the characteristics of the circuit being simulated.
 

Thread Starter

brightnight1

Joined Jan 13, 2018
75
Thanks Crutschow, taking out the timestep increased the speed! One more LT spice question.

I have an LT spice model I would like to use, Part #IRLR7833TRPBF. I found the model, open the text file but the tutorials I found say that the prefix after .model has to be the same as in the standard model I'll be changing in LT spice. I placed an NMOS FET in LTspice but when I look at the prefix next to the text file I downloaded for my part it says "MM NMOS". Can I change the prefix in my LTspice model to MM NMOS or do I have to find a model with the same prefix and what might what be?

This is the text for the part I want to use:



.SUBCKT irlr_u7833 1 2 3
* SPICE3 MODEL WITH THERMAL RC NETWORK
**************************************
* Model Generated by MODPEX *
*Copyright(c) Symmetry Design Systems*
* All Rights Reserved *
* UNPUBLISHED LICENSED SOFTWARE *
* Contains Proprietary Information *
* Which is The Property of *
* SYMMETRY OR ITS LICENSORS *
*Commercial Use or Resale Restricted *
* by Symmetry License Agreement *
**************************************
* Model generated on Nov 27, 02
* MODEL FORMAT: SPICE3
* Symmetry POWER MOS Model (Version 1.0)
* External Node Designations
* Node 1 -> Drain
* Node 2 -> Gate
* Node 3 -> Source
M1 9 7 8 8 MM L=100u W=100u
.MODEL MM NMOS LEVEL=1 IS=1e-32
+VTO=2.40344 LAMBDA=0.0879286 KP=341.2
+CGSO=3.69175e-05 CGDO=1.29046e-06
RS 8 3 0.00360701
D1 3 1 MD
.MODEL MD D IS=2.97198e-13 RS=0.00346153 N=0.887257 BV=30
+IBV=0.00025 EG=1 XTI=1 TT=0.0001
+CJO=1.70357e-09 VJ=1.47001 M=0.507991 FC=0.5
RDS 3 1 1e+06
RD 9 1 0.0001
RG 2 7 2.71931
D2 4 5 MD1
* Default values used in MD1:
* RS=0 EG=1.11 XTI=3.0 TT=0
* BV=infinite IBV=1mA
.MODEL MD1 D IS=1e-32 N=50
+CJO=6.32081e-10 VJ=1.69479 M=0.3 FC=1e-08
D3 0 5 MD2
* Default values used in MD2:
* EG=1.11 XTI=3.0 TT=0 CJO=0
* BV=infinite IBV=1mA
.MODEL MD2 D IS=1e-10 N=0.4 RS=3e-06
RL 5 10 1
FI2 7 9 VFI2 -1
VFI2 4 0 0
EV16 10 0 9 7 1
CAP 11 10 1.9036e-09
FI1 7 9 VFI1 -1
VFI1 11 6 0
RCAP 6 10 1
D4 0 6 MD3
* Default values used in MD3:
* EG=1.11 XTI=3.0 TT=0 CJO=0
* RS=0 BV=infinite IBV=1mA
.MODEL MD3 D IS=1e-10 N=0.4
.ENDS irlr_u7833

*SPICE Thermal Model Subcircuit
.SUBCKT irlr_u7833t 3 0

R_RTHERM1 2 3 0.145
R_RTHERM2 1 2 0.228
R_RTHERM3 0 1 0.28
C_CTHERM1 2 3 0.000814246
C_CTHERM2 1 2 0.003087719
C_CTHERM3 0 1 0.300855

.ENDS irlr_u7833t
 

eetech00

Joined Jun 8, 2013
2,368
The subcircuit should be compatible with LTspice's NMOS symbol.

1. Place the NMOS symbol on the schematic.
2. Mouse-over the symbol then ctl-right click to view the attributes.
3. Change "Prefix" value from MN to X
4. Change "Value" value from NMOS to irlr_u7833
5. Click OK.
6. Point anywhere on schematic then press "t" key to add a "spice Directive".
7. Select the "spice Directive" radio button, then click in the text pane to add the following directive:

.lib filename.ext

This is the filename and extension of the spice model file. Be sure its in the same folder as the schematic.
(You can also browse for the file as well). Then click OK.
The directive will appear in black text by default. If its "blue" you probably didn't select the correct radio button in step 6. above.

That's it.

If you use multiple NMOS transistors of the same type, copy an paste this one to the other locations on the schematic.
Otherwise, you'll have to repeat the above steps for each one.
 
Top