Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Problem in saving data during DC sweep simulation in Cadence Virtuoso

Status
Not open for further replies.

Junus2012

Advanced Member level 5
Joined
Jan 9, 2012
Messages
1,552
Helped
47
Reputation
98
Reaction score
53
Trophy points
1,328
Location
Italy
Activity points
15,235
Dear friends,

I am trying to plot the GBW of my amplifiier under the whole range of the input common mode voltage (VIC). Therefore I run both the DC and AC analyses in the same time, I sweep the VIC from the DC setup from 0 to 3.3 V and from the AC analyses I must get the GBW.

The problem when I run this setting the simulator is not giving me the GBW for every step in VIC, he is ignoring the DC sweep.

I make trick to overcome this problem by sweeping the DC from the parametric analyses, it works fine but it is time consuming.

Can you please suggest me method to fix the problem from DC analyses.

Mr. Suta has already proposed me a solution for similar case but that setting was only to plot the transistor parameters.

Thank you in advance

Best Regards
 

Instead of doing a DC sweep, can you do a transient sweep of your VIC and run .ac at different points (time points which you have to enter by hand) of the transient sweep?
 
DC Analysis is not required.

Simply do parametric sweep for AC analysis from Cadence ADE.
Or enclose ac analysis statement by sweep statement in netlist.
 
Instead of doing a DC sweep, can you do a transient sweep of your VIC and run .ac at different points (time points which you have to enter by hand) of the transient sweep?

Dear Suta,
my supervisor suggested me not to include transient analyses to sweep the VIC, because transient simulation first it takes time and second it shows time behavoural of the circuit which we do not want to include in our basic ac simulation

- - - Updated - - -

DC Analysis is not required.

Simply do parametric sweep for AC analysis from Cadence ADE.
Or enclose ac analysis statement by sweep statement in netlist.

Dear pancho,
Thank you for your reply,

That is actually what I am doing right now, I am sweeping the VIC from parametric, but parametric takes more time than sweeping from DC analyses.
Why sweeping VIC from DC analyses is not connected to ac simulation for every step ? or it is the nature of ADE simulator ?
 

Dear Suta,
my supervisor suggested me not to include transient analyses to sweep the VIC, because transient simulation first it takes time and second it shows time behavoural of the circuit which we do not want to include in our basic ac simulation

- - - Updated - - -


It is true that transient may exercise time behavior of the circuit but this is in case if you change you VIC too fast. If the change is slow enough, then it is pretty much like DC.
 
Show me netlist when you invoke parametric sweep.


Dear Pancho,

The parametric has no problem, it is well working, but I am asking why the simulation fail to present data in grpah if I do the sweep from DC ?

- - - Updated - - -

See the image below to better explain,

you see the graph of the ICMR which I want to have, x-axis is the VIC that I sweep from 0 to 3.3.
AV is the gain I should have from AC simulation

Now the first thing I do is to run the DC and AC simulation together, the AC simulation to find the AV, the DC simulation is to sweep the VIC. This setup fails, the simulator is not running AC for every change in the VIC, he only take one value of VIC (the default value which i put to 1.65 V) then he run the AC simulation on it.

in my second setup I only run the AC simulation, but I sweep the VIC by using the parametric sweep, this configuration is working.

ICMR.jpg

thank you once again again

- - - Updated - - -

It is true that transient may exercise time behavior of the circuit but this is in case if you change you VIC too fast. If the change is slow enough, then it is pretty much like DC.

Dear Suta,

That is the reason why I would like to run it by transient
 

Dear friends,

I recieved an answer from Cadence,

there are two solutions:

1. Simulation using ADE Explorer to set up the surrounding sweep, then spectre would (normally) run with similar efficiency to having a native sweep. That's because it groups the runs and ADE tells spectre to run each set of analyses without quitting the simulator - so you don't need to generate a new netlist, re-start the simulator, regain the license, parse the netlist and so on - spectre will change the parameter value in memory.

Unfortunately my Cadence version is old and not supporting ADE Explorer

2. By making Parametric analyses run faster

check what:

envGetVal("spectre.envOpts" "controlMode")

returns. If that returns "interactive", then doing the parametric sweep should be quick (assuming you're not running in distributed mode in ADE L). If it's set to "batch" then do:

envSetVal("spectre.envOpts" "controlMode" 'string "interactive")

and restart ADE L and try the parametric analysis tool again.
 

1. Simulation using ADE Explorer to set up the surrounding sweep,
then spectre would (normally) run with similar efficiency to having a native sweep.
I don't think so.

Both ADE-XL(GXL) and ADE-Explorer have very large over head.
So multiple sweep simulation speed is very slow compared to Spectre's native sweep ability.

See "spectre -h sweep".
https://www.edaboard.com/showthread.php?387035#3

Unfortunately my Cadence version is old and not supporting ADE Explorer
https://www.edaboard.com/showthread.php?373647
https://www.edaboard.com/showthread.php?381680

Don't rely on Cadence-ADE.
Rather don't use Cadence-ADE.
 
Last edited:
I don't think so.

Both ADE-XL(GXL) and ADE-Explorer have very large over head.
So multiple sweep simulation speed is very slow compared to Spectre's native sweep ability.

See "spectre -h sweep".
https://www.edaboard.com/showthread.php?387035#3


https://www.edaboard.com/showthread.php?373647
https://www.edaboard.com/showthread.php?381680

Don't rely on Cadence-ADE.
Rather don't use Cadence-ADE.

Dear Pancho,
Thank you very much for your nice links,

referring to your statment ''Or enclose ac analysis statement by sweep statement in netlist'', how to implement it? I am not familiar with Ocian in running my simulation, Only I use the GUI of the ADE

To your next statement "Don't rely on Cadence-ADE.
Rather don't use Cadence-ADE"

What you suggest me then to use ?

Thank you very much once again
 

I am not familiar with Ocian in running my simulation
OCEAN is not required.
OCEAN is no more than an assistant of generating netlist.

What you suggest me then to use ?
Excecute simulation from netlist directly as same as HSPICE.

Modifying netlist manually.
You can never utilize full ability of Cadence Spectre as far as you use GUI.
 
Status
Not open for further replies.

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top