QSPICE simulation of LTSPICE netlist runs but nothing appears in output window

QSPICE
1

Hi, I’m a new QSPICE user, trying to simulate an LTSPICE netlist with no luck.
I added missing .lib files and added .plot V(VA), etc. lines to the netlist file.
When I click on the Run button, there are no errors, but nothing shows up in the Output Window.
What am I missing?
I’ve attached my LTSPICE netlist below:

* E:\Users\foo\LTSpice\LED_Driver\Simple_with_Cable_LR_+IR_Limiter\LED_Driver.asc
* Generated by LTspice 26.0.0 for Windows.
VDD VDD 0 5V
VLED VLED 0 PWL(0 0V 1ms 6V)
R1 G N010 47
R2 S 0 1
R3 N002 N003 4
D1 VA VC 1N4007
C1 N003 0 470µF V=10 Irms=1.4 Rser=0.1 Lser=0 mfg="Vishay" pn="T97H477M010" type="Tantalum Conf Coat"
R4 NIDAQ_AO N012 40.2K
R5 N012 0 10K
D2 0 N012 1N4148
C2 N012 0 10pF
C4 N014 0 220nF
R6 G N014 10
VSRC NIDAQ_AO 0 PULSE(0V 5V 50ms 1us 1us 100us 10ms)
C3 N010 N009 1pF
L1 N003 N007 1.1µH
X§U2 VC G S FET_TEMP FDT439N ;§pnba D)G)S)T
R7 N007 VA 0.65
R8 N011 N004 100
X§U1 N011 N009 VDD 0 N010 VDD ADA4805 ;§pnba 100)101)102)103)104)106
R9 N008 N004 100
X§U3 N008 0 VDD 0 NC_01 VDD ADA4805 ;§pnba 100)101)102)103)104)106
R10 N006 N004 100
X§U4 N006 0 VDD 0 NC_02 VDD ADA4805 ;§pnba 100)101)102)103)104)106
R11 N005 N004 100
X§U5 N005 0 VDD 0 NC_03 VDD ADA4805 ;§pnba 100)101)102)103)104)106
R12 N004 0 1G
R13 S N009 6.8K
X§U6 N012 N004 VDD 0 N004 ADA4084-2 ;§pnba In+)In-)V+)V-)OUT
C5 N003 0 470µF V=10 Irms=1.4 Rser=0.1 Lser=0 mfg="Vishay" pn="T97H477M010" type="Tantalum Conf Coat"
C6 N003 0 470µF V=10 Irms=1.4 Rser=0.1 Lser=0 mfg="Vishay" pn="T97H477M010" type="Tantalum Conf Coat"
C7 N003 0 470µF V=10 Irms=1.4 Rser=0.1 Lser=0 mfg="Vishay" pn="T97H477M010" type="Tantalum Conf Coat"
R14 N002 N003 4
R15 N002 N003 4
R16 N002 N003 4
R17 VLED N002 2
X§U7 N002 N001 VLED NC_04 NDT456P ;§pnba D)G)S)T
R18 N001 VLED 100K
R19 0 N001 20K
C8 VLED N001 1µF V=10 Irms=1.4 Rser=0.1 Lser=0 mfg="Vishay" pn="T97H477M010" type="Tantalum Conf Coat"
.model D D
.lib C:\Users\techie\AppData\Local\LTspice\lib\cmp\standard.dio
.option ITL4=200 Gmin=1e-11 Abstol=1e-10 Trtol=4 Chgtol=1e-10 MinDeltaGmin=0.0001
*.options cshunt=1e-15
.ic V(C1)=0 V(C5)=0 V(C6)=0 V(C7)=0 V(C8)=0
.tran 70ms uic
* Differential Loop Inductance = 220nH / ft.\nof 28AWG twisted pair wires w/\n0.8mm spacing.
* BAC: 5ft. max.\ncable length
* NI DAQ slew rate = 5V/us
* AD8605:\n1K, 47, 33nF\n33, 12, 470nF\n \nADA4805:47, 10, 220nF
* 28AWG Cable Resistance =  0.065 Ohms / ft.\nRloop = 0.13 Ohms / ft.
* 10V::2A\n5V::1A
* Chgtol must be >= 1e-10 for stability
* Series Current Limiting Resistor\ncharges flash cap in 5*tau = 10ms
* Library below included based on ModelFile attribute of instance X§U6 (C:\Users\techie\AppData\Local\LTspice\lib\sym\OpAmps\ADA4084-2.asy)
.lib ADA4084-2.lib
* Library below included based on ModelFile attribute of instance X§U1, X§U3, X§U4, X§U5 (C:\Users\techie\AppData\Local\LTspice\lib\sym\OpAmps\ADA4805.asy)
.lib ADI.lib
* Library below included based on ModelFile attribute of instance X§U2 (E:\Users\techie\Vivonics\Active Projects\2160 BAC PhII\POC\LTSpice\LED_Driver\Simple_with_Cable_LR_+IR_Limiter\FDT439N.asy)
.lib FDT439N.ckt
* Library below included based on ModelFile attribute of instance X§U7 (E:\Users\techie\Vivonics\Active Projects\2160 BAC PhII\POC\LTSpice\LED_Driver\Simple_with_Cable_LR_+IR_Limiter\NDT456P.asy)
.lib NDT456P.ckt
.plot V(VA), V(VC)
.backanno
.end
2

Hi, 2Torr.

I’m unsure exactly how you’re trying to run this from the QSpice GUI. Please upload the schematic.

You’re a new user so see this post: Qspice Forum - New User to Basic User (File Upload) - QSPICE - Qorvo Tech Forum

Edit: If you want to run a netlist directly, enter the following in a command prompt window:

"c:\program files\qspice\qspice64.exe" test2.cir

Where test2.cir is the netlist. If successful, this will generate test2.qraw which you can double-click in File Explorer to open in the Waveform viewer. If not successful, you’ll get error messages that may help identify the problem.

–robert

3

@RDunn I expected @2Torr to run this netlist and encounter errors reported in the output window, but according to his description, this is not the case. In his netlist, he calls multiple LTspice libraries and his own library (FDT439N.lib and NDT456P.ckt), and for example, ADA4084-2.lib from LTspice contains LTspice A-device which is unique for LTspice and cannot be run in Qspice. But the strange thing is that he got nothing showing up in the Output Window instead of multiple errors. However, having only the netlist will not help us in replicating his issue; we also need his own libraries. I expect at least these 3 files are required to be upload to seek for help : LED_Driver.cir, FDT439N.ckt, NDT456P.ckt

4

Thanks for the helpful replies!
I forgot to mention that I was first getting an error about the unsupported A device, so I downloaded a SPICE macro model (ADA4084.cir) from ADI’s website with no A devices, then simply renamed it to ADA4084-2.lib. Then when I ran QSPICE I received no messages.
It turns out that the original ADA4084-2.lib file has a top subcircuit named ADA4084-2, while the
downloaded ADA4084.cir has a top subcircuit named ADA4084 instead. It’s strange that QSPICE didn’t give me an error that a model for the ADA4084-2 was not found…

Next, I changed the netlist to use ADA4084 instance (instead of ADA4084-2) and included ADA4084.cir and ADA4805.cir (part of ADI.lib, too big to include here) instead.
Now, when I run QSPICE, I receive a warning for a singular matrix, asking me to check node 82 in the ADA4084 macro model. I reported this issue to ADI.

Finally, I was able to get the simulation to run by removing the ‘uic’ in the .tran statement.

As a new user, I’m not allowed to upload files, and I don’t have the time right now to copy and paste long netlists into the editor. Thanks again for all the help!

1 Like