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.

Register Log in

Cadence Spectre - DC Analysis after Transient

Status
Not open for further replies.
K

kishore2k4

Full Member level 5
Full Member level 5
Joined
Jun 17, 2006
Messages
291
Helped
44
Reputation
88
Reaction score
11
Trophy points
1,298
Location
Middle Earth
Activity points
3,295
The following is for a Bandgap circuit simulation.
How can I set spectre to do DC analysis only after the VDD (vpwl) is completely ramped up. The transient simuation shows proper response but the DC analysis is being performed at t=0 which happened to be Vdd=0.

I tried setting the order in Setup -> Environment but it has no effect.
 

In spectre each voltage source typiccaly has parameter "DC voltage" this voltage will be used by DC simulation. Set this voltage to what it needs to be.
 

    K

    kishore2k4

    Points: 2
    Helpful Answer Positive Rating
monya11 said:
In spectre each voltage source typiccaly has parameter "DC voltage" this voltage will be used by DC simulation. Set this voltage to what it needs to be.
Click to expand...

Thank You, I tried it but that didn't work in this case. The error amp is (self)-biased from the bandgap, unless DC-Analysis can wait till the currents have properly settled the simulation output is going to be wrong. Any advice?
 

kishore2k4 said:
monya11 said:
In spectre each voltage source typiccaly has parameter "DC voltage" this voltage will be used by DC simulation. Set this voltage to what it needs to be.
Click to expand...

Thank You, I tried it but that didn't work in this case. The error amp is (self)-biased from the bandgap, unless DC-Analysis can wait till the currents have properly settled the simulation output is going to be wrong. Any advice?
Click to expand...

DC analyses have no time properties.
Therefore my advice: Do a tran analysis instead using a linear voltage ramp of the corresponding source. This analysis can be delayed by a time specified by you.
 

    K

    kishore2k4

    Points: 2
    Helpful Answer Positive Rating
LvW said:
kishore2k4 said:
monya11 said:
In spectre each voltage source typiccaly has parameter "DC voltage" this voltage will be used by DC simulation. Set this voltage to what it needs to be.
Click to expand...

Thank You, I tried it but that didn't work in this case. The error amp is (self)-biased from the bandgap, unless DC-Analysis can wait till the currents have properly settled the simulation output is going to be wrong. Any advice?
Click to expand...

DC analyses have no time properties.
Therefore my advice: Do a tran analysis instead using a linear voltage ramp of the corresponding source. This analysis can be delayed by a time specified by you.
Click to expand...

I can do that but I have one small problem(I think). I am using one of those capacitor startup circuits that turns itself off when the circuit is biased properly. The only way (I know of) to trigger that startup circuit is with a varying(ramp, however short it may be) voltage on the supply line. Is there any other way around this? Thanks.

PS: I think the main issue is with the use of this particular startup rather than other things.
 
  • Like
Reactions: erikl

    erikl

    erikl

    Points: 2
    Helpful Answer Positive Rating
Perhaps you want to use a different source for your power
supply - for example, a vpulse lets you set the DC voltage
to one value, but transient initial and pulse values to something
else (so, DC=3V, tran initial=0, tran pulse=3, etc.).

Or, you could not insist on running all the analyses with the same
variables and conditions and schematic base.
 

kishore2k4 said:
I think the main issue is with the use of this particular startup rather than other things.
Click to expand...
Also, with your transient analysis you could use the writefinal option, which writes the last oppoint info to a file, and then start your DC analysis with the prevoppoint option, which then uses the previously stored oppoint info from the transient analysis.
 
Thank You for all the replies. The problem has been rectified.

erikl said:
Also, with your transient analysis you could use the writefinal option, which writes the last oppoint info to a file, and then start your DC analysis with the prevoppoint option, which then uses the previously stored oppoint info from the transient analysis.
Click to expand...

The method suggested by erikl did the job, with one small change. I couldn't get DC analysis to take prevoppoint ( I understand that it is mainly used for small-signal (AC, stb etc) analysis? ). What I did was to use the writefinal option in Transient analysis and read that file using readns in DC-Analysis options.

Also one may want to set skipdc=yes in transient analysis.
 
kishore2k4 said:
What I did was to use the writefinal option in Transient analysis and read that file using readns in DC-Analysis options.
Click to expand...
Thank you, kishore,
for reporting back your successful implementation!
Also for having clicked helped me! ;-)
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top