SPICE (LT): determining dissipation by resistors, etc.?

[Mike Rocket J. Squirrel Elliott]

Newbie question:

What's the quick and easy way of finding the steady-state power
dissipation of resistors and other components in a circuit with SPICE?

..op gives me node voltage and device currents and, yep, I could do the
simple math. How can I get SPICE to do it?

 

[Mike Engelhardt]

Mike,

What's the quick and easy way of finding the steady-state
power dissipation of resistors and other components in a
circuit with SPICE?

.op gives me node voltage and device currents and, yep,
I could do the simple math. How can I get SPICE to do it?

In LTspice, device power is only computed as part of an
efficiency calculation in a .tran analysis, but since
efficiency is only computed for SMPS's in steady state,
it isn't of much use for general simulations.

The easiest way to enter the simple math to plot the power
dissipation of a resistor in a general simulation in LTspice
is to do a .tran analysis and then drag the cross-probe cursor
across the resistor so that now the differential voltage is
plotted. Then right click on the plot label say, V(a,b),
and edit it 1K*V(a,b), or what ever value of resistance you
have.

--Mike

 

[Jim Thompson]

Mike,


In LTspice, device power is only computed as part of an
efficiency calculation in a .tran analysis, but since
efficiency is only computed for SMPS's in steady state,
it isn't of much use for general simulations.

The easiest way to enter the simple math to plot the power
dissipation of a resistor in a general simulation in LTspice
is to do a .tran analysis and then drag the cross-probe cursor
across the resistor so that now the differential voltage is
plotted. Then right click on the plot label say, V(a,b),
and edit it 1K*V(a,b), or what ever value of resistance you
have.

--Mike

Does LTSpice have "avg" and "avgx" functions like PSpice?

If so, you can display the averaged power.

...Jim Thompson

 

[Helmut Sennewald]

Mike,


In LTspice, device power is only computed as part of an
efficiency calculation in a .tran analysis, but since
efficiency is only computed for SMPS's in steady state,
it isn't of much use for general simulations.

The easiest way to enter the simple math to plot the power
dissipation of a resistor in a general simulation in LTspice
is to do a .tran analysis and then drag the cross-probe cursor
across the resistor so that now the differential voltage is
plotted. Then right click on the plot label say, V(a,b),
and edit it 1K*V(a,b), or what ever value of resistance you
have.

Hello Mike,
something like V(a,b)*V(a,b)/10k is ok for DC, but what if I have
a time dependent voltage V(a,b). I will need an integration of P(t)
over time.
Is there any hidden(not documented) command for integration?

I would like something as s(...) .
PROBE in PSPICE has this function.

Best Regards
Helmut

 

[Mike Engelhardt]

I miswrote:

...Then right click on the plot label say, V(a,b),
and edit it 1K*V(a,b), or what ever value of resistance you
have....

Opps, wasn't thinking, you would then edit it to read V(a,b)*I(R1)
to get instantaneous power.

--Mike

 

[Mike Engelhardt]

Does LTSpice have "avg" and "avgx" functions like PSpice?

something like V(a,b)*V(a,b)/10k is ok for DC, but what

Opps, sorry for the mistake.

if I have a time dependent voltage V(a,b). I will need an
integration of P(t) over time. > Is there any hidden(not
documented) command for integration?

After you plot the instanteneous power with I(R1)*V(a,b)
then you can integrate it to get the average and rms
values by holding down the control key and left clicking on
the plot trace's label. You control integration limits with
the horizontal zoom of the plot. This Control-click to
integrate gives different types of integrations for different
analysis types. It will integrate noise in quadrature after a
..noise analysis. It will give bandwidths after a .ac analysis.

Sorry again about writting 1K*V(a,b) instead of I(R1)*V(a,b)
for power. The method can be used for devices with more
than two pins. For the power in a bipolar transistor,
plot V(b)*Ib(Q1)+V(c)*Ic(Q1)+V(e)*Ie(Q1) Where V(b), V(c),
and V(e) are base, collector, and emitter voltages.

--Mike

 

[Paul Burridge]

Does LTSpice have "avg" and "avgx" functions like PSpice?

If so, you can display the averaged power.

Jim, you need to dump PSpice *immediately* and get a copy of LT.
Trust me. I know what I'm talking about. I think.
No, seriously! LT is *all* you need. Why pay oodles of dollars when
you don't need to?
Screw P.

 

[Mike Rocket J. Squirrel Elliott]

Mike,




In LTspice, device power is only computed as part of an
efficiency calculation in a .tran analysis, but since
efficiency is only computed for SMPS's in steady state,
it isn't of much use for general simulations.

The easiest way to enter the simple math to plot the power
dissipation of a resistor in a general simulation in LTspice
is to do a .tran analysis and then drag the cross-probe cursor
across the resistor so that now the differential voltage is
plotted. Then right click on the plot label say, V(a,b),
and edit it 1K*V(a,b), or what ever value of resistance you
have.

To me, it's surprising that SPICE doesn't generate as a matter of
course, the steady-state Pd for parts along with the usual voltage drop
and current. But hey! I just want to make sure I order resistors big
enough for the job -- I expect that the folks that create SPICEs seldom
worry about that, or it would be part of the package.

Thanks for the tip!

 

[Helmut Sennewald]

Opps, sorry for the mistake.


After you plot the instanteneous power with I(R1)*V(a,b)
then you can integrate it to get the average and rms
values by holding down the control key and left clicking on
the plot trace's label. You control integration limits with
the horizontal zoom of the plot. This Control-click to
integrate gives different types of integrations for different
analysis types. It will integrate noise in quadrature after a
.noise analysis. It will give bandwidths after a .ac analysis.

Hello Mike,
thanks for the tipp.
I will remmeber always to try the powerful <control> key in the
future if I miss some feature.

Best Regards
Helmut

 

[andy thompson]

Hi Mike,

In Micro-Cap you plot PD(R1) (PD for power dissipated), where R1 is
the name of the resistor. This essentially plots I(R1)^2*R(R1). You
can also plot ED(R1) to see the energy dissipated during the run. To
see average power you could use the AVG (average) function as in

AVG(PD(R1))

You can get a demo version of Micro-Cap at www.spectrumn-soft.com.

Cheers,

Andy Thompson

 

[Jim Thompson]

Hi Mike,

In Micro-Cap you plot PD(R1) (PD for power dissipated), where R1 is
the name of the resistor. This essentially plots I(R1)^2*R(R1). You
can also plot ED(R1) to see the energy dissipated during the run. To
see average power you could use the AVG (average) function as in

AVG(PD(R1))

You can get a demo version of Micro-Cap at www.spectrumn-soft.com.

Cheers,

Andy Thompson

[snip]

Gawwwd! Can't even correctly spell his own website ;-)

...Jim Thompson

 

[qrk]

Jim, you need to dump PSpice *immediately* and get a copy of LT.
Trust me. I know what I'm talking about. I think.
No, seriously! LT is *all* you need. Why pay oodles of dollars when
you don't need to?

Graphing. PSpice has a few more graphing goodies than LTSpice offers.
I find the Performance Analysis feature in PSpice to be very handy.

Node voltage and device current annotation on the schematic. Don't
know if LTSpice has this, but this sure is handy when trying to debug
stuff.

No, I'm not trashing LTSpice. I'm quite partial to LTSpice, especially
since Mike is so responsive getting bugs fixed and adding features.
When the graphing gets tough, gotta switch to PSpice.

Mark

 

[Jim Thompson]

Graphing. PSpice has a few more graphing goodies than LTSpice offers.
I find the Performance Analysis feature in PSpice to be very handy.

Node voltage and device current annotation on the schematic. Don't
know if LTSpice has this, but this sure is handy when trying to debug
stuff.

No, I'm not trashing LTSpice. I'm quite partial to LTSpice, especially
since Mike is so responsive getting bugs fixed and adding features.
When the graphing gets tough, gotta switch to PSpice.

Mark

Same here. Some of us have to do this for a living. (Actually LOVE
to do this for a living... can't EVER pass up a challenge ;-)

...Jim Thompson

 

[Mike Engelhardt]

Mark, Jim,

Same here. Some of us have to do this for a living. (Actually LOVE
to do this for a living... can't EVER pass up a challenge ;-)

Yes, PSpice does still have more plotting features than
LTspice, but LTspice has some that PSpice doesn't have.
For example, in LTspice, you can sweep a parameter at a
single frequency as in this deck:

*
I1 0 1 ac 1
L1 1 0 100u
R1 1 0 100K
C1 1 0 {C}
..step oct param C 200p 300p 500
..ac list 1Meg
..end

Similarly, you can plot noise density at a single
frequency vs. a parameter. There'll be more plotting
features added to LTspice before the end of the year.
Also, LTspice handles waveform data in a 64bit address
space so the waveform files are unlimited in size.
Designers find it more viable for doing full-chip,
transistor-level simulations not only because of
it's vastly superior solving capabilities over PSpice,
but also because of it's improved data-handling for
large data sets.

--Mike

 

[Kevin Aylward]

Hi Mike,

In Micro-Cap you plot PD(R1) (PD for power dissipated), where R1 is
the name of the resistor. This essentially plots I(R1)^2*R(R1). You
can also plot ED(R1) to see the energy dissipated during the run. To
see average power you could use the AVG (average) function as in

In SuperSpice, you move the mouse over the component, dc power and ave.
tran power is shown bottom right of main window. That's it, its all
automatic. Oh, also, you just put a test point on the component to plot
its power.

Kevin Aylward
[email protected]
http://www.anasoft.co.uk
SuperSpice, a very affordable Mixed-Mode
Windows Simulator with Schematic Capture,
Waveform Display, FFT's and Filter Design.

 

[Paul Burridge]

Yes, PSpice does still have more plotting features than
LTspice, but LTspice has some that PSpice doesn't have.
For example, in LTspice, you can sweep a parameter at a
single frequency as in this deck:

*
I1 0 1 ac 1
L1 1 0 100u
R1 1 0 100K
C1 1 0 {C}
.step oct param C 200p 300p 500
.ac list 1Meg
.end

Is this a new feature, Mike? I wasn't aware that LT had this highly
useful capability.

 

[Mike Engelhardt]

Paul,

Is this a new feature, Mike? I wasn't aware that LT had this highly
useful capability.

As I remember, it was there as part of the first release of LTspice
that supported .step. That became a documented feature on
Jan 8, 2002. An example of doing this for in a .noise simulation
is in ./examples/Educational/stepnoise.asc. There you can see
the diff pair tail resistance that gives the lowest input referenced
noise density.

--Mike

 

[andy thompson]

Hi All,

The correct web site for the Micro-Cap demo is:

www.spectrum-soft.com

Thanks to Jim Thompson for noticing this and pointing it out.

Cheers,

Andy Thompson

Hi Mike,

In Micro-Cap you plot PD(R1) (PD for power dissipated), where R1 is
the name of the resistor. This essentially plots I(R1)^2*R(R1). You
can also plot ED(R1) to see the energy dissipated during the run. To
see average power you could use the AVG (average) function as in

AVG(PD(R1))

You can get a demo version of Micro-Cap at www.spectrumn-soft.com.

Cheers,

Andy Thompson

[snip]

Gawwwd! Can't even correctly spell his own website ;-)

...Jim Thompson

 

[analog]

Hi All,

Hi Andy

The correct web site for the Micro-Cap demo is:

www.spectrum-soft.com

It's a beautiful site (gotta love your newsletters), but why would
any serious designer in their right mind pay thousands of dollars
for your software when they can get LTspice with its superior core
functionality for free? (not just a rhetorical question, btw)

LTspice surely by now must be noticeably eroding your market share
and reducing your revenues. What is your strategy for dealing
with this? Are you planning price reductions or perhaps cutting a
licensing deal so that one of Linear Technology's competitors can
offer a free simulator? Maybe National Semiconductor would be
interested.

Thanks to Jim Thompson for noticing this and pointing it out.

No thanks needed, I'm sure. Pointing out the foibles of others is
one of his pleasures. -- analog

 

[Mike Engelhardt]

Mike,

What's the quick and easy way of finding the steady-state power
dissipation of resistors and other components in a circuit with SPICE?

There's a new feature in version 2.07a. From a schematic,
you can now plot the instantaneous power dissipation in a
device. This is accessed by Alt-Left clicking on a symbol.
It's computed as an expression of voltages and currents
that are already in the data set. For example, if you
Alt-click on a transistor, the trace you add might look
like "V(N001,N003)*Ic(Q1)+V(N002,N003)*Ib(Q1)" Average
power dissipation can be found by control clicking
on this trace label to integrate.

--Mike