Error When trying to Import the subcircuit Spice model into Cadence

Hi Matt,

That blog was written many years ago.  There's a more up-to-date version on Cadence Online Support FAQ: How to Include a Subcircuit (Netlist) into a Schematic and Simulate in ADE 

Do you have access to https://support.cadence.com ?

What version of Virtuoso are you using?   This command (typed in a linux window) will give that information:

virtuoso -W

Thanks,

Tawna

Hi Matt,

That blog was written many years ago.  There's a more up-to-date version on Cadence Online Support FAQ: How to Include a Subcircuit (Netlist) into a Schematic and Simulate in ADE 

Do you have access to https://support.cadence.com ?

What version of Virtuoso are you using?   This command (typed in a linux window) will give that information:

virtuoso -W

Thanks,

Tawna

Tawna, 

Thanks for your quick reply. Unfortunately, I do not have access to the link and cadence community support. I have previously also contacted Cadence for getting the access but they mentioned only school liasons have the access, not the students. 

I am using 6.1.7.64b.500.18 version. 

Regards,

Mehdi

Hi Matt, 

Sorry for the late reply.  Looks like I need to rewrite the blog.  :-)   

Your university should be able to connect you with the "university liason" (typically the professor) who can download the article for you.  The article is now written for IC6.1.8 and ICADVM 20.1 (so there may be some slight differences compared to IC6.1.7).  

You can also use the "SPICEIn" (virtuoso → File → Import → Spice) feature to import netlists and create schematics.  I believe that was available in IC6.1.7 (I don't remember).

For me to assist, it would be helpful if you showed us your process step by step.  I may see something obvious that you are forgetting to do.   

Sorry, I'm taking off for the evening and won't be near my computer.  

best regards,

Tawna

From the symptoms described, the most likely problem that the view name you gave the spectreText view you created is not included in the switch view list.

So, assuming that the view name was "spectreText", go to Setup->Environment in ADE and for the "view list" field, add "spectreText" at the beginning of the list. This is the list of views to try when traversing the hierarchy.

Using a spectre text view avoids the need to create a stopping view, or to need to edit the CDF using the approach covered in Tawna's blog. It also means you don't need to include the text of the subckt using the Setup->Model Libraries or Setup->Simulation Files, as the netlister will automatically reference the definition in the spectreText view.

Andrew.

Thanks to both of you for your help. Our school liaison forwarded the instructions to me and it works fine, but I do have an error now: 

Error found by spectre during initial setup.
    ERROR (CMI-2078): spice: Required parameter `file' is missing.

So is that error from when you ran the simulation? Did it give other error info that said which line of which file it had a problem with? Perhaps you could post the entire log file (you can attach files to the forum post)?

Andrew

Sure. Here is the whole log file for your reference, I have added the Spice model as well which is available online: 

This is the log file:

Cadence (R) Virtuoso (R) Spectre (R) Circuit Simulator
Version 15.1.0.803.isr18 64bit -- 21 Jun 2017
Copyright (C) 1989-2017 Cadence Design Systems, Inc. All rights reserved worldwide. Cadence, Virtuoso and Spectre are registered trademarks of Cadence Design Systems, Inc. All others are the property of their respective holders.

Includes RSA BSAFE(R) Cryptographic or Security Protocol Software from RSA Security, Inc.

User: mehdina94rm   Host: 08vlab089   HostID: 5A0A5908   PID: 18430
Memory  available: 170.6188 MB  physical: 16.8257 GB
Linux   : CentOS Linux release 7.7.1908 (Core)
CPU Type: Intel(R) Xeon(R) CPU E5-2698 v4 @ 2.20GHz
All processors running at 2200.0 MHz
        Socket: Processors
        0:       0,  1
        1:       2,  3
       
System load averages (1min, 5min, 15min) : 20.5 %, 14.2 %, 10.0 %
This is a virtual machine


Simulating `input.scs' on 08vlab089 at 4:39:14 PM, Tue Mar 23, 2021 (process id: 18430).
Current working directory: /ECEnet/home/student/mehdina94rm/Sim/PAD115_tb/spectre/schematic/netlist
Command line:
    /ECEnet/Apps1/linux/cad12/tools/cadence/MMSIM151/tools/bin/spectre  \
        -64 input.scs +escchars +log ../psf/spectre.out -format psfxl  \
        -raw ../psf +lqtimeout 900 -maxw 5 -maxn 5

Loading /ECEnet/Apps1/linux/cad12/tools/cadence/MMSIM151/tools.lnx86/cmi/lib/64bit/5.0/libinfineon_sh.so ...
Loading /ECEnet/Apps1/linux/cad12/tools/cadence/MMSIM151/tools.lnx86/cmi/lib/64bit/5.0/libphilips_o_sh.so ...
Loading /ECEnet/Apps1/linux/cad12/tools/cadence/MMSIM151/tools.lnx86/cmi/lib/64bit/5.0/libphilips_sh.so ...
Loading /ECEnet/Apps1/linux/cad12/tools/cadence/MMSIM151/tools.lnx86/cmi/lib/64bit/5.0/libsparam_sh.so ...
Loading /ECEnet/Apps1/linux/cad12/tools/cadence/MMSIM151/tools.lnx86/cmi/lib/64bit/5.0/libstmodels_sh.so ...
Reading file:  /ECEnet/home/student/mehdina94rm/Sim/PAD115_tb/spectre/schematic/netlist/input.scs
Reading file:  /ECEnet/Apps1/linux/cad12/tools/cadence/MMSIM151/tools.lnx86/spectre/etc/configs/spectre.cfg
Reading file:  /ECEnet/Apps1/linux/cad12/tools/cadence/MMSIM151/tools.lnx86/spectre/etc/configs/mapsubckt.cfg
Reading file:  /Users/Grad/mehdina94rm/Desktop/PAD115.ckt
Time for NDB Parsing: CPU = 150.786 ms, elapsed = 333.993 ms.
Time accumulated: CPU = 204.021 ms, elapsed = 334.006 ms.
Peak resident memory used = 38.1 Mbytes.


The CPU load for active processors is :
        Spectre  0 (18.8 %)      1 (63.6 %)      2 (18.8 %)      3 (18.8 %)
        Other  
Reading link:  /ECEnet/Apps1/linux/cad12/tools/cadence/MMSIM151/tools.lnx86/spectre/etc/ahdl/discipline.h
Reading file:  /ECEnet/Apps1/linux/cad12/tools/cadence/MMSIM151/tools.lnx86/spectre/etc/ahdl/disciplines.vams
Reading link:  /ECEnet/Apps1/linux/cad12/tools/cadence/MMSIM151/tools.lnx86/spectre/etc/ahdl/constants.h
Reading file:  /ECEnet/Apps1/linux/cad12/tools/cadence/MMSIM151/tools.lnx86/spectre/etc/ahdl/constants.vams

Warning from spectre in `PAD115':`I0', during hierarchy flattening.
    WARNING (SFE-30): "/Users/Grad/mehdina94rm/Desktop/PAD115.ckt" 125: I0.JA: `NR' is not a valid parameter for an instance of `jfet'.  Ignored.
    WARNING (SFE-30): "/Users/Grad/mehdina94rm/Desktop/PAD115.ckt" 125: I0.JA: `VK' is not a valid parameter for an instance of `jfet'.  Ignored.

Time for Elaboration: CPU = 42.777 ms, elapsed = 62.3231 ms.
Time accumulated: CPU = 247.213 ms, elapsed = 396.742 ms.
Peak resident memory used = 44.3 Mbytes.


Warning from spectre during hierarchy flattening.
    WARNING (CMI-2049): I0.QP1: Value of `ikr' should be greater than zero.  Ignored.

Time for EDB Visiting: CPU = 4.287 ms, elapsed = 5.48005 ms.
Time accumulated: CPU = 251.877 ms, elapsed = 402.598 ms.
Peak resident memory used = 45.1 Mbytes.


Warning from spectre during initial setup.
    WARNING (CMI-2318): I0.Q11: Parasitic resistor `rc' has been deleted because its value of 80 mOhm ( R / MFactor ) was smaller than `minr'.
    WARNING (CMI-2318): I0.Q11: Parasitic resistor `re' has been deleted because its value of 80 mOhm ( R / MFactor ) was smaller than `minr'.
    WARNING (CMI-2318): I0.Q10: Parasitic resistor `rc' has been deleted because its value of 80 mOhm ( R / MFactor ) was smaller than `minr'.
    WARNING (CMI-2318): I0.Q10: Parasitic resistor `re' has been deleted because its value of 80 mOhm ( R / MFactor ) was smaller than `minr'.
    WARNING (CMI-2318): I0.Q9: Parasitic resistor `rc' has been deleted because its value of 80 mOhm ( R / MFactor ) was smaller than `minr'.
        Further occurrences of this warning will be suppressed.
    WARNING (CMI-2316): I0.X5.D3: Parasitic resistor `rs' has been deleted because its value of 3 uOhm ( R / (Area * MFactor) ) was smaller than `minr'.
    WARNING (CMI-2316): I0.X4.DSD: Parasitic resistor `rs' has been deleted because its value of 11.5 mOhm ( R / (Area * MFactor) ) was smaller than `minr'.
    WARNING (CMI-2316): I0.X3.DSD: Parasitic resistor `rs' has been deleted because its value of 11.5 mOhm ( R / (Area * MFactor) ) was smaller than `minr'.
Notice from spectre during initial setup.
    I0.X5.MM: Default value for `uo' is used.
    I0.X5.MM: Values of `kp' and `uo' are not consistent.
    I0.X3.DMOS: Default value for `uo' is used.
    I0.X3.DMOS: Values of `kp' and `uo' are not consistent.
    I0.X3.DMOS: `cgso' is not specified.  0.1um * Cox is used.
    I0.X3.DMOS: `cgdo' is not specified.  0.1um * Cox is used.
Error found by spectre during initial setup.
    ERROR (CMI-2078): spice: Required parameter `file' is missing.


Aggregate audit (4:39:14 PM, Tue Mar 23, 2021):
Time used: CPU = 255 ms, elapsed = 406 ms, util. = 62.8%.
Time spent in licensing: elapsed = 36.3 ms, percentage of total = 8.95%.
Peak memory used = 45.6 Mbytes.
Simulation started at: 4:39:14 PM, Tue Mar 23, 2021, ended at: 4:39:14 PM, Tue Mar 23, 2021, with elapsed time (wall clock): 406 ms.
spectre completes with 1 error, 16 warnings, and 6 notices.
spectre terminated prematurely due to fatal error.

Spice Model:

* POWER AMP DESIGN PAD115 High Voltage High Power Op Amp

*Note: Operational amplifiers are often difficult to converge in SPICE
*because of the high gain of the amplifier. To assist convergence it
*is often helpful to nodeset the -IN node and the OUT node to the voltage
*expected. Also, it is helpful to set options for ITL1 to 10000, ITL2 to 2500
*and ITL4 to 2500.
*Note: shutdown function and temperature output are not simulated.
*Note: Vcc is connected to +Vs, -Vcc is connected to -Vs
*V1.1 Oct 9 2006

*    

simulator lang=spice

**

spice macro subckt netlist

  *                         -IN +IN CC1 CC2 +VS -VS  OUT
.SUBCKT PAD115    1     2     3       4       5      6      10
 

*** CONTENT REMOVED BY MODERATOR TO AVOID DISCLOSING COPYRIGHTED/PROPRIETARY INFORMATION
       
 .ENDS

Dear MattNEU,

1. Perhaps it my misunderstanding of your post, but you've included the following line in your SPICE model file:

simulator lang=spice

but it is not the first line in the file. I am not sure - Andrew will know - but I do not believe spectre recognizes the SPICE comment character as a comment. Since it is not the first line, this may cause a problem when spectre reads in the file.

Did you try placing the line "simulator lang=spice" as the very first line of the file?

2. How and where did you include the path to your spice model file? You need to include the full pathname and enclose it in double-quotes. The most typical place to include it is in your Model file setup GUI.

Shawn

I removed the content of the SPICE Model above because it was not clear that you were allowed to post it in a public forum (it said it contained proprietary information, so it would have been better to reference where it was published elsewhere rather than posting the file here in case you're breaking copyright).

Anyway, the issue is due to this line:

spice macro subckt netlist

That''s not a valid SPICE line, and so you should put a "*" at the beginning of the line to make it a comment. If you do that, it will proceed without the error.

To answer 's concern, Spectre also copes with the SPICE comment syntax of using * at the beginning of a line, so the simulator lang doesn't need to be at the beginning. Anyway, the file appears to have a suffix of ".ckt" so would have been treated as SPICE syntax anyway, so the simulator lang=spice is superfluous.

Andrew