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

Mike Rocket J. Squirrel E · Oct 31, 2003

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 "Rocket J Squirrel" Elliott

Mike Engelhardt · Oct 31, 2003

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 · Oct 31, 2003

On 31 Oct 2003 19:28:54 GMT, "Mike Engelhardt" <pmte@concentric.net>
wrote:

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

480)460-2350 | |
| E-mail Address at Website Fax

Helmut Sennewald · Oct 31, 2003

"Mike Engelhardt" <pmte@concentric.net> schrieb im Newsbeitrag
news:bnud5m$j3v@dispatch.concentric.net...

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.

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 · Oct 31, 2003

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 · Oct 31, 2003

Jim wrote:

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

Helmult wrote:

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 · Oct 31, 2003

On Fri, 31 Oct 2003 13:06:08 -0700, Jim Thompson
<invalid@invalid.invalid> wrote:

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.

--

"Windows [n.], A thirty-two bit extension and GUI shell to a sixteen bit patch
to an eight bit operating system originally coded for a four bit
microprocessor and produced by a two bit company."

Mike Rocket J. Squirrel E · Oct 31, 2003

Mike Engelhardt wrote:

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.

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!

--
Mike "Rocket J Squirrel" Elliott

Helmut Sennewald · Oct 31, 2003

"Mike Engelhardt" <pmte@concentric.net> schrieb im Newsbeitrag
news:bnujup$qvp@dispatch.concentric.net...

Jim wrote:

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

Helmult wrote:

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.

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 · Oct 31, 2003

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

"Mike Engelhardt" <pmte@concentric.net> wrote in message news:<bnud5m$j3v@dispatch.concentric.net>...

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 · Nov 1, 2003

On 31 Oct 2003 15:58:19 -0800, andy@spectrum-soft.com (andy thompson)
wrote:

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]

480)460-2350 | |
| E-mail Address at Website Fax

qrk · Nov 1, 2003

On Fri, 31 Oct 2003 21:40:22 +0000, Paul Burridge
<pb@osiris.notthisbit.co.uk> wrote:

On Fri, 31 Oct 2003 13:06:08 -0700, Jim Thompson
invalid@invalid.invalid> wrote:

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?

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 · Nov 1, 2003

On Fri, 31 Oct 2003 17:55:35 -0800, qrk <mark@reson.DELETE.ME.com>
wrote:

On Fri, 31 Oct 2003 21:40:22 +0000, Paul Burridge
pb@osiris.notthisbit.co.uk> wrote:

On Fri, 31 Oct 2003 13:06:08 -0700, Jim Thompson
invalid@invalid.invalid> wrote:

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?

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

480)460-2350 | |
| E-mail Address at Website Fax

Mike Engelhardt · Nov 1, 2003

Mark, Jim,

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?

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.

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 · Nov 1, 2003

andy thompson wrote:

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
salesEXTRACT@anasoft.co.uk
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 · Nov 1, 2003

On 01 Nov 2003 04:36:14 GMT, "Mike Engelhardt" <pmte@concentric.net>
wrote:

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.
--

"Windows [n.], A thirty-two bit extension and GUI shell to a sixteen bit patch
to an eight bit operating system originally coded for a four bit
microprocessor and produced by a two bit company."

Mike Engelhardt · Nov 1, 2003

Paul,

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.

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 · Nov 1, 2003

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

Jim Thompson <invalid@invalid.invalid> wrote in message news:<s2u5qv03dgqgriemipaf0cchl3a4flo2lq@4ax.com>...

On 31 Oct 2003 15:58:19 -0800, andy@spectrum-soft.com (andy thompson)
wrote:

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
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| Phoenix, Arizona Voice480)460-2350 | |
| E-mail Address at Website Fax480)460-2142 | Brass Rat |
| http://www.analog-innovations.com | 1962 |

I love to cook with wine. Sometimes I even put it in the food.

analog · Nov 1, 2003

Andy Thompson wrote:

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

Cheers,

Andy Thompson

Mike Engelhardt · Nov 18, 2003

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

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

Mike Rocket J. Squirrel E

Guest

Mike Engelhardt

Guest

Jim Thompson

Guest

Helmut Sennewald

Guest

Mike Engelhardt

Guest

Mike Engelhardt

Guest

Paul Burridge

Guest

Mike Rocket J. Squirrel E

Guest

Helmut Sennewald

Guest

andy thompson

Guest

Jim Thompson

Guest

qrk

Guest

Jim Thompson

Guest

Mike Engelhardt

Guest

Kevin Aylward

Guest

Paul Burridge

Guest

Mike Engelhardt

Guest

andy thompson

Guest

analog

Guest

Mike Engelhardt

Guest

Log in

Welcome to EDABoard.com

Sponsor