Designer’s Guide Community

Mariusz New Member Offline Posts: 5	Temperature Simulation Aug 18^th, 2009, 1:51pm Does anyone know how to run a transient simulation over time and at some point change the temperature. I would like to see the response to a temperature change over time. This is a temperature sensor circuit and I am using spectre.
Back to top	IP Logged

Andrew Beckett

Senior Fellow

Offline

Life, don't talk to
me about Life...

Posts: 1742
Bracknell, UK

Re: Temperature Simulation
Reply #1 - Aug 19^th, 2009, 5:30am

Code:

tran1 tran stop=0.5u param=temp param_vec=[0 20 50n 25] param_step=0

which will have the temperature at 20 degrees until 50ns when it will change to 25. Or:

Code:

tran1 tran stop=0.5u param=temp param_vec=[0 20 50n 25] param_step=10n

This will take 10ns steps between �the temperature values at 0s and 50ns, so will rise by 1 degree every 10ns.

In ADE the param, param_vec, param_step fields do not appear (yet) on the tran analysis options form, so you'll need to type these parameters in the "Additional Parameters" field at the bottom of the tran options form.

This capability was added in MMSIM62, so you'll need to use a version of spectre which is MMSIM62 or later.

Generally I would advise against taking too big a temperature change in one go because this potentially could lead to convergence difficulties as you suddenly introduced a big discontinuity into the simulation (and of course, that would be completely unrealistic).

Best Regards,

Andrew.

Back to top

IP Logged

Mariusz New Member Offline Posts: 5	Re: Temperature Simulation Reply #2 - Aug 19^th, 2009, 6:00am Thank you very much. This is exactly what I was looking for and it works great!!!!!!!!!!
Back to top	IP Logged

ahmadyan

New Member

Offline

Posts: 1
Iran

Re: Temperature Simulation
Reply #3 - Sep 9^th, 2009, 7:06am

I want to do the similar simulation, do you know this kind of transient simulation for hsim?
I tried to get this spectre netlist to hsim but it doesn't support this kind of param.

Andrew Beckett wrote on Aug 19^th, 2009, 5:30am:

Code:

tran1 tran stop=0.5u param=temp param_vec=[0 20 50n 25] param_step=0

which will have the temperature at 20 degrees until 50ns when it will change to 25. Or:

Code:

tran1 tran stop=0.5u param=temp param_vec=[0 20 50n 25] param_step=10n

This will take 10ns steps between �the temperature values at 0s and 50ns, so will rise by 1 degree every 10ns.

In ADE the param, param_vec, param_step fields do not appear (yet) on the tran analysis options form, so you'll need to type these parameters in the "Additional Parameters" field at the bottom of the tran options form.

This capability was added in MMSIM62, so you'll need to use a version of spectre which is MMSIM62 or later.

Generally I would advise against taking too big a temperature change in one go because this potentially could lead to convergence difficulties as you suddenly introduced a big discontinuity into the simulation (and of course, that would be completely unrealistic).

Best Regards,

Andrew.

Back to top

IP Logged

Andrew Beckett Senior Fellow Offline Life, don't talk to me about Life... Posts: 1742 Bracknell, UK	Re: Temperature Simulation Reply #4 - Sep 10^th, 2009, 5:26am I can't answer, as I don't have access to hsim. But you might want to try reading (or searching) the hsim documentation. I would imagine that if it is supported, it's documented somewhere... Regards, Andrew.
Back to top	IP Logged

Andrew Beckett Senior Fellow Offline Life, don't talk to me about Life... Posts: 1742 Bracknell, UK	Re: Temperature Simulation Reply #5 - Sep 10^th, 2009, 5:30am And BTW, for spectre, it's now in the ADE tran analysis GUI, since 5.10.41.500.6.138. I think for IC613 it will be in 6.1.3.500.14. Regards, Andrew.
Back to top	IP Logged