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

[SOLVED] What‘s wrong with the simulation result of the very basic RC circuit

Status
Not open for further replies.
I

iamyuchenjie

Junior Member level 1
Joined
Aug 3, 2009
Messages
16
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Location
Germany
Activity points
1,429
Solved （Cadence）What‘s wrong with the simulation result of the very basic RC circuit

Hallo,
I'm an EE student from TU Dresden.
Today I try to simulate some very basic RC circuits. （In spectre of Cadence 5141）
I am totally confused with the results. For example, I drew a very basic source-free RC serial circuit and try to find it's transient response. The circuit is as follow:
schematic.png
But the simulation result is that： the voltage of net3 start from (time 0 ) is 12.5V, instead of the initial condition value I set15V？
sim-result.png
And I also try some other circuits with cap. but all the result is not right according to my understanding. I asked in the edabord, but no reply up to now.
Do you know why? I think the cap from the analoglib (Cadence build-in lib)is the ideal one, isn't it?
Or can u simulate it for me? Just 5 minutes is quite enough I think.
Really thank you！

--------------------------------------------------------------------------------
 
Last edited:

Hallo,
I'm an EE student from TU Dresden.
Today I try to simulate some very basic RC circuits.
I am totally confused with the results. For example, I drew a very basic source-free RC serial circuit and try to find it's transient response. The circuit is as follow:

But the simulation result is that： the voltage of net3 start from (time 0 ) is 12.5V, instead of the initial condition value I set15V？

And I also try some other circuits with cap. but all the result is not right according to my understanding. I asked in the edabord, but no reply up to now.
Do you know why? I think the cap from the analoglib (Cadence build-in lib)is the ideal one, isn't it?
Or can u simulate it for me? Just 5 minutes is quite enough I think.
Really thank you！
Click to expand...
Hi iamyuchenjie
I can simulate it for you . but if you want i simulate something for you , mention the required parameters as well .
Best Wishes
Goldsmith
 

Thanks Goldsmith！
All the parmeters are here:a 0.1f ideal capacitor with initial condition of v(0)=15V
a resistier of 1 Ohm.
I want to simulate the de-charing process of the cap.
But in my environment, I get the result that the voltage across the cap. changes from 12V instead of 15V at the start! It seems to violate the circuits theory.
 

Thanks Goldsmith！
All the parmeters are here:a 0.1f ideal capacitor with initial condition of v(0)=15V
a resistier of 1 Ohm.
I want to simulate the de-charing process of the cap.
But in my environment, I get the result that the voltage across the cap. changes from 12V instead of 15V at the start! It seems to violate the circuits theory.
Click to expand...
Hi again
Ok here result of my simulations comes :



Any question ?
Good Luck
Goldsmith
 

iamyuchenjie said:
But in my environment, I get the result that the voltage across the cap. changes from 12V instead of 15V at the start! It seems to violate the circuits theory.
Click to expand...

Did you see what would happen if you start it at 17V? It's worth a try.

This is one of those situations where a simulator does something erroneous, for reasons unknown. We are forced to try any kind of workaround that we can.

After using the simulator a while something may become clear. You may figure out what settings let you use your original plan. Maybe adjusting the time step? Etc.

For the time being, you may as well do the same thing you would do with real components. Charge up the capacitor from a power source, then switch it over to a resistor. Command the scope to display the entire process.

For a view of how another simulator does it, here is my screenshot of Falstad's simulator. I see Goldsmith already did something similar. Mine lacks scale readings.

 

Thank you all.

I have tried everything I can try in the simulator---spectre of Candence ic5141.
One thing to point is when I adjust the value of resist much lager, then the result come close to the theory value. But I still don't know why?
Cadence, I am disappointed with your performance this time。。。:sad:

BradtheRad said:
Did you see what would happen if you start it at 17V? It's worth a try.

This is one of those situations where a simulator does something erroneous, for reasons unknown. We are forced to try any kind of workaround that we can.

After using the simulator a while something may become clear. You may figure out what settings let you use your original plan. Maybe adjusting the time step? Etc.

For the time being, you may as well do the same thing you would do with real components. Charge up the capacitor from a power source, then switch it over to a resistor. Command the scope to display the entire process.

For a view of how another simulator does it, here is my screenshot of Falstad's simulator. I see Goldsmith already did something similar. Mine lacks scale readings.

Click to expand...
 

Try with the "Use Initial Conditions" option on i.e.
.TRAN 0 1 UIC
Click to expand...
I am not quite sure what the simulator does during the operating point calculation if UIC is not used, but my guess is that it places a voltage source with 1 ohm resistance at the Initial Condition node. That affects the starting point it arrives at. By specifying UIC it doesn't calculate the operating point at all and so starts the transient analysis with the values specified.

Keith
 

Thank you！
Your analysis is reasonable.
But where can I set the Use Initial Conditions in cadence？
What is i.e.....
Can you give me more detail information?
I use cadence icfb 5141.
Thank you very much!
keith1200rs said:
Try with the "Use Initial Conditions" option on i.e. I am not quite sure what the simulator does during the operating point calculation if UIC is not used, but my guess is that it places a voltage source with 1 ohm resistance at the Initial Condition node. That affects the starting point it arrives at. By specifying UIC it doesn't calculate the operating point at all and so starts the transient analysis with the values specified.

Keith
Click to expand...
 

I don't use Cadence so I cannot help with the specifics of how you set it. It will be in the transient analysis setup and may be called something like "skip DC bias point calculation". Your Cadence "help" system may give the answer.

Keith
 

keith1200rs said:
...but my guess is that it places a voltage source with 1 ohm resistance at the Initial Condition node. ...
Click to expand...

Looks like that. It is as if a 1 Ω resistance were used to set the initial condition only, not as a part of the model of the capacitor:
The time constant of the discharge is exactly 0.4 s, i.e. 0.1 F with 4 Ω, not (4+1) Ω .
 

I checked it with various values to confirm that was the case. With 1V and 1 ohm you get 0.5V on the capacitor which confirms the extra 1 ohm. Provided you use the UIC option it is fine. I use SIMetrix and it also has a method of setting the initial voltage on a capacitor without using UIC, but that is not the standard SPICE method.

Keith
 

keith1200rs said:
I checked it with various values to confirm that was the case. With 1V and 1 ohm you get 0.5V on the capacitor which confirms the extra 1 ohm. Provided you use the UIC option it is fine. I use SIMetrix and it also has a method of setting the initial voltage on a capacitor without using UIC, but that is not the standard SPICE method.

Keith
Click to expand...

Thank you Keith, you are so talent! Dein intuition ist really gut!!!
Thank you all the friends above!
I like the forum!
 

Presumed the assumption of a 1 ohm series resistor for initial condition voltage sources is true, it should be mentioned somewhere in the manuals. Otherwise cadence support must know about.

1 Ohm sounds unusually high, maybe reasonable though for IC design, the primary Cadence domain. The high value makes me think there could be a system parameter to modify it.

Pspice uses 0.2 milliohm with .IC commands B.T.W.:

During bias calculations, PSpice clamps the voltages to specified values by attaching a voltage source with a 0.0002 ohm series resistor between
the specified nodes. After the bias point has been calculated and the transient analysis started, the node is released.
Click to expand...
 
FvM said:
Presumed the assumption of a 1 ohm series resistor for initial condition voltage sources is true, it should be mentioned somewhere in the manuals. Otherwise cadence support must know about.

1 Ohm sounds unusually high, maybe reasonable though for IC design, the primary Cadence domain. The high value makes me think there could be a system parameter to modify it.

Pspice uses 0.2 milliohm with .IC commands B.T.W.:
Click to expand...

You are right.
And I find that in Cadence after reading the spectre reference, this parameter name “rforce”.
 

I looked in SIMetrix and Hspice manuals but didn't find a parameter but will check 'rforce' tomorrow.

Keith
 

I find the parameter in the Spectre Circuit Simulator Reference Product Version 5.0 September 2003, and near the part of transient analysis
 

I couldn't find it in Hspice but in SIMetrix it is ICRES. Also found this
If the UIC parameter is absent from the .TRAN control then a DC operating point is
calculated before the transient analysis. In this case the net voltages specified on the
.IC control are forced to the desired initial values during the DC operating point
solution. Once transient analysis begins this constraint is released. By default the
voltage force is effectively carried out via a 1Ω resistor. This can be changed with the
option setting ICRES.
Click to expand...

Keith
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top