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.

How to do dc sweep 2 variables input in cadence spectre

Status
Not open for further replies.

tompham

Full Member level 2
Joined
May 29, 2010
Messages
133
Helped
29
Reputation
60
Reaction score
29
Trophy points
1,308
Location
usa
Activity points
2,066
Hi all

Anyone know how to run cadence spectre with sweeping 2 input variables? Let say sweep vgs and vds of nmos

Thank your
 

pancho_hideboo

Advanced Member level 5
Joined
Oct 21, 2006
Messages
2,856
Helped
766
Reputation
1,532
Reaction score
722
Trophy points
1,393
Location
Real Homeless
Activity points
17,469
Use nested sweep analysis.
Code:
swp_vds sweep param=vds start=0 stop=1.5 step=0.1 {
    swp_vgs sweep param=vgs start=0 stop=0.5 step=0.1 {
         .......
    }
}

See result "spectre -h sweep".
 
Last edited:

tompham

Full Member level 2
Joined
May 29, 2010
Messages
133
Helped
29
Reputation
60
Reaction score
29
Trophy points
1,308
Location
usa
Activity points
2,066
Hi pancho_hideboo

Where I can add the lines you mention? In input.scs? and after adding the lines I need to run not to netlist and run?

Thanks
 

pancho_hideboo

Advanced Member level 5
Joined
Oct 21, 2006
Messages
2,856
Helped
766
Reputation
1,532
Reaction score
722
Trophy points
1,393
Location
Real Homeless
Activity points
17,469
Cadence Spectre have multiple sweep analyses using sweep analysis.
See "spectre -h dc" and "spectre -h sweep".

If you run Spectre simulation from Unix Command line such as "spectre input.scs".
You can use following analysis statement.
Code:
swp_vds sweep param=vds start=0 stop=1.5 step=0.1 {
    swp_vgs dc param=vgs start=0 stop=0.5 step=0.1 {
         .......
    }
}

However it can not be available directly, if you run Spectre from Cadence ADE.
You can specify vgs sweep as dc native sweep from ADE.
However you can not set sweep analysis for vds from ADE.

Instead you can use Parametric Analysis for vds sweep.
This is ADE function not Spectre function.
ADE's Ocean generates input.scs with changing vds.
This is equivalent to the following.
Code:
spectre input_vds1.scs
spectre input_vds2.scs
   ....
   ....
spectre input_vds_N.scs

You can not use full ability of Spectre if you run it from ADE.
 
Last edited:

april1975

Member level 2
Joined
Nov 11, 2011
Messages
49
Helped
2
Reputation
4
Reaction score
2
Trophy points
1,288
Activity points
1,588
Hello
pancho_hideboo Wrote:
You can not use full ability of Spectre if you run it from ADE.
Is there quick start guide documents to learn full ability of spectre?
tnx
 

april1975

Member level 2
Joined
Nov 11, 2011
Messages
49
Helped
2
Reputation
4
Reaction score
2
Trophy points
1,288
Activity points
1,588
Hello pancho
I googled for
Virtuoso Spectre Circuit Simulator and Accelerated Parallel Simulator User Guide
, and I found:
Spectre Circuit Simulator User Guide
which have 334 pages. Is it what you have mentioned?
 

dick_freebird

Advanced Member level 5
Joined
Mar 4, 2008
Messages
7,510
Helped
2,169
Reputation
4,344
Reaction score
2,058
Trophy points
1,393
Location
USA
Activity points
60,050
Every time I had to do nested loops, I used the Parametric
Analysis tool and a DC OP. You may not find any value in
a continuous sweep. You -could- run Spectre native or
under Ocean, but if you are in the graphical environment
maybe you'd rather get to the outcome and skip the voyage
of discovery. Unless said voyage is the point of it all.
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top