AnalogLib VDC with DC = 0V and transient noise has an clear average of <> 0V

Dear Fabian,

df03sch said:

During my online search I found out that the exact same problem was already reported in Cadence_Forum but the question got closed without any solutions and that the only user who responded is not longer a member of the forum.

I am still participating in the Forum. For some unknown reason to Cadence, all of my posts in the past were renamed from my name to the name "Former member". I was told they would correct it, but that was 6 months ago.

df03sch said:

When performing a transient analysis with transient noise enabled of a single vdc source from the analog-lib with VDC = 0V and one single noise pair the average output voltage is not equal to VDC = 0V as there is a voltage jump after the first simulation step. This means at t = 0 the output voltage is at 0mV, but with the first transient simulation point the output jumps for several mV and stays at this value while the applied noise is then in the order of a few 100uV (peakToPeak). I'm even seeing a difference on the simulation time, meaning the dc offset after the first simulation step shifts with different transient simulations times. 

I understand you have difficulty providing results on the Forum, but can you include text such as you netlist, noise file, input.scs, runSimulation line and tool versions? You mentioned:

df03sch said:

the issue seen and the used setup (GND + VDC from analog-lib) is the same as in the above reported link.

However, the noise file, netlist, input.scs and runSimulation line are different as well as your tool version. Did you try to duplicate the exact simulation example included in the Forum post at URL:

https://community.cadence.com/cadence_technology_forums/f/custom-ic-design/52249/voltage-jump-in-transient-noise-simulation-when-reading-data-from-file

You should be able to duplicate the results I include as I've included the netlist, input.scs, and noise file. You could even copy the input.scs file and noise file and run them from the spectre command. If you want, I have the noise file, input.scs file and netlist files and can provide them to you. You should be able to duplicate the results in the note.

Shawn

Hi Shawn,

thanks for replying and good to hear that you're still on the topic. 

Unfortunately I can't open the dropbox link caused by the companies security settings (I just had a look at the pdf via my smartphone) and didn't saw any big differences. However, I was running the exact same circuit where I saw the issue in the secure-net on a unsecure-net with a different camino version and there the problem wasn't visible.

Input.scs 

simulator lang=spectre
global 0
include "netlist"
simulatorOptions options psfversion="1.4.0" reltol=1e-3 vabstol=1e-6 \
iabstol=1e-12 temp=27 tnom=27 scalem=1.0 scale=1.0 gmin=1e-12 rforce=1 \
maxnotes=5 maxwarns=5 digits=5 cols=80 pivrel=1e-3 \
sensfile="../psf/sens.output" dochecklimit=yes checklimitdest=both
tranCheckLimit checklimit checkallasserts=yes severity=none
tran tran stop=25u errpreset=conservative noisefmax=1G noiseseed=1 \
write="spectre.ic" writefinal="spectre.fc" annotate=status maxiters=5
primitives info what=primitives where=rawfile
subckts info what=subckts where=rawfile
designParamVals info what=parameters where=rawfile
asserts info what=assert where=rawfile
save V_out
saveOptions options save=selected

Netlist

simulator lang=spectre
V0 (0 V_out) vsource dc=0 type=dc noisevec=[ 20M 1p ]

I compared the input.scs and netlist file visually (as they are quite small), there is no difference. However, the difference in the runs is the used Virtuoso version:

The dc-shift is visible in Spectre 21.1.0.389.isr8 / ICADVM20.1-64b.500.25.EHF11261

The dc-shift is not visible in Spectre 20.1.0.186.isr5 / IC6.1.8-64b.500.17 and Spectre 19.1.0.348.isr6 / IC6.1.8-64b.500.13.EHF7868

Please notice that the faulty DC-shift is visible in the newest spectre version from the 3 used combinations. 

As I can't attach any pictures from the secure net: The average from the signal V_out is equal to 19.61mV while the (clipped) peakToPeak is 17.22mV. The first lines of the .csv-output with the relevant DC-jump at the first transient-simulation step is:

Dear Fabian,

Thank you for following through on this and all your added information!

df03sch said:

Unfortunately I can't open the dropbox link caused by the companies security settings (I just had a look at the pdf via my smartphone) and didn't saw any big differences.

I understand. Our company had the same block. I do have access to OneDrive, and if you still need to access it outside of your smartphone, I can place it there or send it to you. Nonetheless, it appears you are satisfied with the comparison between our settings and input files. I also looked at your input.scs and netlist and do not see anything that appears significantly different. The one item not clear from your last note is what version of the spectre simulator you are using. For example, are you using spectre, spectre +aps, or spectre ++aps? Since you have an errpreset of conservative, I assume you are not running spectre X. This information can be found in the runSimulation file contained in your netlist directly. spectre (without its +aps nor ++aps options) is the "golden standard", and hence you might try a run using just pure spectre.

df03sch said:

However, I was running the exact same circuit where I saw the issue in the secure-net on a unsecure-net with a different camino version and there the problem wasn't visible.

df03sch said:

The dc-shift is visible in Spectre 21.1.0.389.isr8 / ICADVM20.1-64b.500.25.EHF11261

The dc-shift is not visible in Spectre 20.1.0.186.isr5 / IC6.1.8-64b.500.17 and Spectre 19.1.0.348.isr6 / IC6.1.8-64b.500.13.EHF7868

That was a good experiment! The version I used was

Version 20.1.0.382.isr12 64bit -- 5 Nov 2021

and I did not observe the offset. I checked back to the Forum post at URL:

https://community.cadence.com/cadence_technology_forums/f/custom-ic-design/52249/voltage-jump-in-transient-noise-simulation-when-reading-data-from-file

but the Forum poster did not include the version he or she used.

At this point, I think you need to open a support ticket with Cadence. They will want a test case to verify they can reproduce your result - and you already have that! I no longer have access to the Cadence tools and hence cannot verify your result with 21.1.0.389.isr8 - sorry!

Good work Fabian!

Shawn

Hi Shawn,

thanks for you answer, I already tested all three basic versions (Spectre/APS/SpectreX) in the opening post... I didn't try to rerun the tests with the different versions but I don't think that it is related to the simulator, more a problem of the vdc itself. I will get in contact with the local DAE to issue to support ticket to Cadence.

I keep you updated

Greetings

Fabian

Dear Fabian,

df03sch said:

I already tested all three basic versions (Spectre/APS/SpectreX) in the opening post...

Thank you for the added information! I do see you included that in your initial post and forgot - sorry! As a side note in case you were no aware of it, there is a difference between spectre +aps and spectre ++aps.

df03sch said:

I will get in contact with the local DAE to issue to support ticket to Cadence.

Perfect Fabian! I appreciate it. I think you have found an issue and hopefully it will result in an update soon. if you have an account with Cadence, you can also open a ticket yourself.

Shawn