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

One question of hspice/spectre simulation?

Status
Not open for further replies.
G

GaryHan

Newbie level 5
Joined
Mar 3, 2004
Messages
8
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
74
When I do trans simulation, i wann to change a cap value during the simulation, not restart the simulation, but in the simulation to see the parameter of the cap influence the result?
How can i do using the hspice or spectre in the analog artist? Thx 8)

Maybe I don't speak it clearly, I give you an example.
A cap is used as a sensor, it can be changed by the circumstance. i can do the simulation with different value, but during one simulation the value of the cap is fixed, not a variable. i want to give 5p to the cap at the beginning of the simulation, and change it to 10p at 500us and recover it to 5p at 1ms. That will give you a strange result rather than give it a constant value. How can i do? Please give me some advise! Thx
 

i think u can do it by parameter sweep commands
 

In HSPICE you can define the capacitance of a capacitor with an equation. For example:

Csensor node1 node2 c='5p*v(controlvoltage)' CTYPE=1

This will make your capacitor depend on the voltage at the node "controlvoltage". If this voltage is defined to be 1V from 0s to 500us, 2V from 500us to 1ms and back to 1V at 1ms, this will do what you want.

The "CTYPE" option controls the charge calculation method and needs to be "1" if the capacitance is supposed to vary with node voltages (the default value is "0").

Regards
 

I do not know what is useable in Hspice but in most spice you be limited to a nonlinear cap. So the control voltage is the cap voltage themselve. I think you have to use an analog behaviour with an integration function and a multiplier or a function for the integration time constant.
 

In HSPICE you do not have such limitation... The example I gave is almost a copy of what is in the manual...

Regards
 

I checked spectre.

The instance definition of capacitor does not include an external voltage or node definition for the nonlinear cap.
 

In HSPICE you can define the capacitance of a capacitor with an equation. For example:

Csensor node1 node2 c='5p*v(controlvoltage)' CTYPE=1

This will make your capacitor depend on the voltage at the node "controlvoltage". If this voltage is defined to be 1V from 0s to 500us, 2V from 500us to 1ms and back to 1V at 1ms, this will do what you want.

The "CTYPE" option controls the charge calculation method and needs to be "1" if the capacitance is supposed to vary with node voltages (the default value is "0").

Regards


This method is very useful, and I have already solve my difficulties by using this method. Thank you, maxwellequ.
Click to expand...
 

You can build a ideal voltage controlled capacitor model using Spectre verilog or Verilog A, and then just change the control voltage during simulation. it is very simple. But you need to use spectre.
 

How to build a ideal voltage controlled capacitor model using Spectre verilog or Verilog A?
Can you describe it in detail? Thx a lot!
 

Use capacitors in parallel with ideal switches in series from the AnalogLib.

Enable and disable the switches as you see fit during the simulation.


for instance switch in a 5 pF cap with the 5pF already in there.
and at a later time switch it out using a control signal generated separately.

Hope this helps.
 

You can write an ideal model of your capacitor with Verilog-A, then run the simulation.
 

u can implement two or more caps on paralell conection and turn them off or turn them on. i don`t know if sources will help u to do it
 

In Spectre you can do it with using the sweeps command. You can change a value as part of a sweep, but after each change another simulation iteration is done. In Spectre this can be done without killing and restarting the simulation process. Switching a parallel capcitor in using an ideal switch is probably the easiest solution though.
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top