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

How to add temperature sweep in tran simulation?

Status
Not open for further replies.
P

Pipeline

Advanced Member level 4
Joined
Dec 7, 2004
Messages
118
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,296
Activity points
875
spectre temperature variable in tran

In other words, I'd like to simulate a circuit's performance over temperature at time=20ns or 100 ns.
thanks a lot!
 

spectre temperature sweep in transient analysis

You can save op at time=20ns or 100ns during tran simulation, then do the temp sweep to use these op!
I think you can try this method!
 

ac analysis sweep temperature

babbage said:
You can save op at time=20ns or 100ns during tran simulation, then do the temp sweep to use these op!
I think you can try this method!
Click to expand...

How to do?
Can you give us detail description?
Thanks!
 

hspice manual says that very clear
 

you can look up the control statement: .op
such as
.op 100n
 

For Analog Artist, you can setup a trient analysis and do a parameter analysis, then plot the values at 20ns and 100ns.

For hspice, you can use TEMP as the second sweep var in transient analysis. Use .measure statement to get the values at 20ns and 100ns.
 

thanks!
But I do not know how to add a parameter analysis in tran analysis in Spectre using Graphic user interface.
 

Pipeline said:
thanks!
But I do not know how to add a parameter analysis in tran analysis in Spectre using Graphic user interface.
Click to expand...

On your case (you want do transient analysis while sweep temperature), you should use "Parameter Analysis" tool.

1. setup the transient as usual.
2. Select menu "Parameter Analysis" from "Tools" sub-menu.
3. Set the Variable name of Sweep1 to "TEMPDC". You can also get this name by menu: Setup / Pick Name for Variable / Sweep 1...
4. Fill in the other fields and choose menu "Analysis / Start".

If you want to plot the node voltage of net VOUT at time 20ns and 100ns, you can setup the Outputs (in ADE window) as following:
1. Select menu "Outputs / Setup ..."
2. Set Name to VOUT@20ns ( can be anything)
3. Set Expression to value(VT("/VOUT"), 20n)
4. Click "Add" to add the expresion.
5. Define VOUT@100ns in the same way.
 

    P

    Pipeline

    Points: 2
    Helpful Answer Positive Rating
OK, THANKS A LOT!
 

I have one more question.
I also want to check its AC performance, but I cannot use the same mothed to do an AC analysis in transient sim. Would you please give me a favor? thanks!
 

You can use the same method as in transient analysis except the output setup. You can use VF to replace VT. For example, cross(dB20(VF("/OUT")), 0, 1, "falling") will give the unit-gain bandwidth of an opamp.
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top