[SI-LIST] Re: Hspice Network Analysis
- From: Bill.Cohen@xxxxxxxxxxxxxxxx
- To: "Mike Degerstrom" <degers@xxxxxxxxxxxxxxxxxxxx>
- Date: Thu, 13 Nov 2003 10:59:16 -0500
Mike,
I'll check the bias conditions. I just assumed that if the transistor
channel is on that the capacitance won't vary. I'll be more precise and see
if this helps.
We're interested in the resistance of the capacitor. We simulated using
ideal caps and there was resonance between the package and the decoupling
capacitors. Once we put in the spice model for the capacitor the resonance
was suppress by the effective series resistance.
Best Regards,
--------------------------------------------------------------
| Bill Cohen
| Toshiba America Electronic Components
| Mixed Signal Design Group
--------------------------------------------------------------
"Mike Degerstrom"
<degers@advancedsi To:
Bill.Cohen@xxxxxxxxxxxxxxxx, si-list@xxxxxxxxxxxxx
design.com> cc:
Subject: Re: [SI-LIST] Hspice
Network Analysis
11/13/2003 09:42
AM
Bill,
The capacitance is dependant on bias voltage.
This should work:
1) Repeat your transient analysis with a ramp
starting at .9*VDD and stopping at 1.1*VDD.
2) Repeat your AC analysis but with the DC
voltage set to VDD.
Your results now should match. Your analysis is interesting as
I've modeled PDS on chips in the past. I didn't take the time
to see if series resistance makes a difference for on-chip
decaps but suspected it didn't. I actually didn't model
the decaps but used ideal capacitors to match the databook
specs. for the capacitance per sq/micron for the decap
cells.
Mike
On Wed November 12 2003 2:54 pm, Bill.Cohen@xxxxxxxxxxxxxxxx wrote:
> I have been analyzing on chip decoupling capacitors using hspice. I have
> extracted the capacitance of the decoupling capacitor using transient
> analysis. I ramped a voltage (slow Ramp 1ms) and looked for the current.
I
> found the capacitance using the formula
>
> c=i*dt/dv
>
> Using AC analysis I then curve fit an external resistance to mimic my
> routing and transistor channel resistance using a reference ideal RC
> circuit.
>
> I then used the AC Network analysis package available in Hspice. I got
good
> correlation to the resistance but I have bad correlation between the
> capacitance. Does anyone have experience with the Network analysis
> available in Hspice? Why would the Network analysis capacitance number
vary
> widely from the transient analysis? I curve fit from 100K to 1Ghz and ran
> the network analysis at the same frequencies.
>
> Transient Analysis: C=18.6pF
> AC curve fitting of R=2.8 ohms
>
> Network analysis: R=2.86ohms, C=7.95pF.
>
> --------------------------------------------------------------
>
> | Bill Cohen
> | Toshiba America Electronic Components
>
> --------------------------------------------------------------
>
>
> -------------------------------------
--
Mike Degerstrom email: degers@xxxxxxxxxxxxxxxxxxxx
Advanced Signal Integrity Design, LLC http://www.advancedsidesign.com
Phone: 507-289-2900 Fax: 507-280-0052 Cell Phone: 507-254-4448
316 6th Street SW; Rochester, MN 55902
------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
or to administer your membership from a web page, go to:
//www.freelists.org/webpage/si-list
For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
List technical documents are available at:
http:/www.si-list.org
List archives are viewable at:
//www.freelists.org/archives/si-list
or at our remote archives:
http://groups.yahoo.com/group/si-list/messages
Old (prior to June 6, 2001) list archives are viewable at:
http://www.qsl.net/wb6tpu
Other related posts:
