Re: Sub circuit heat dissipation not showing

#90126

Brad,

One of the frustrating things for me about this conversation, is that
I don't think you have made clear what you are simulating, and what
your problem or question is.

You referred to a TIP142 test circuit that (I think) is in the group's
Files area.  So I found it (two copies, they are identical, both named
"TIP142_test.zip") and downloaded and ran it.  So far, so good.  It
would have helped me, if you pointed to that file and said "This is
the thing I am simulating."  Sorry, but with 100+MB of Files here, and
a wealth of SPICE stuff elsewhere on the Internet, and unknown what's
on your computer, it can be tricky to guess what you mean.

I had some trouble trying to find what you quoted that says, "Left
click to plot Q10 dissipation. V(c10)*Ix(Q10:C)+V(b10)*Ix(Q10:B)".  I
guess what you are referring to, is what happens when you
press-and-hold the Alt key, and hover the mouse over the Q10 symbol.
That text appears as a tip in the lower left corner of LTspice.

Yes, LTspice shows you a formula.  It shows you the formula that
LTspice will use when you click there -- the formula that calculates
the power dissipation of Q10.

OK, so now click the mouse button.

Voila -- a plot appears in the waveform window.  That squiggly plot is
a plot of the quantity V(c10)*Ix(Q10:C)+V(b10)*Ix(Q10:B), which equals
the sum of powers into Q10.  In other words, it is the power absorbed
by Q10.  It even goes negative at points -- showing when the device
(through stored charge) is delivering energy back to the external
circuit.

Step back for a moment and remember what's happening.  LTspice just
did a time-domain simulation.  It knows all the currents and all the
voltages, and all the things that depend on currents and voltages, AS
A FUNCTION OF TIME.  All those quantities are functions of time, and
they are known moment-by-moment.

So what is it that you are looking for?

I guess you are looking for the AVERAGE power dissipation of
transistor Q10.  Am I right?

Power dissipation, like voltage and like current, is a function of
time.  Remember that.

So this is where that second thing I referred to previously, comes in
handy.  Go to the Help page for "Waveform Viewer -> Data Trace
Selection", and scroll down almost half way, until you reach the
paragraph between the 3rd and 4th figures on that page, which reads as
follows:

"Yet another schematic probing technique is to plot the instantaneous
power dissipation of a component. To do this, hold down the Alt key
and click on the body of the symbol of the component. The
instantaneous power dissipation will be plotted as an expression of
voltages and currents. It will be plotted on its own scale with the
units of Watts. The mouse cursor turns into an icon that looks like a
thermometer when it's pointing at a dissipation that can be plotted.
You can find the average power dissipation by control-clicking the
trace label."

See that last sentence?  "You can find the average power dissipation
by control-clicking the trace label."

OK, so press-and-hold the Ctrl key, and click the mouse (left button)
on the label at the top of the waveform window -- yes, the one with
that formula.

A little pop-up window appears, showing, among other things, that the
Average power is 41.034 mW.

That is the average power over this interval of time in the plot
window.  It is important to make sure the time interval is meaningful.
If your signals are periodic, you will want to make sure the time
interval corresponds to an exact whole number of cycles.  And check
that nothing "funny" happens, say, at the very start of the simulation
(let's say, if the plotted thing shoots up to 50W for a very brief
moment, but never does that again).

I *think* this is the answer to your question?

Later, you wrote:

   "Interestingly, I noticed that R2 said "dissipation = 0" but when I
plot it I see about 850 mW for about 50 us at 50% duty cycle."

It took me a minute to find what you are referring to.

LTspice shows a bunch of things in its lower left corner, depending on
what it knows, and what it thinks you want to do.  When you hover the
mouse pointer near a net or wire, LTspice shows you the voltage on the
wire, at t=0, and only at t=0.  It can only show you the voltage at
t=0 because the voltage is changing as a function of time.  Right?

The value at t=0 is useful to many people because it is the "operating
point" solution.  In the early days of SPICE, just finding the
operating point alone was a major accomplishment.  Once you knew the
operating point, you could tell most everything about how the circuit
worked.

When you hover the mouse over a resistor, it shows you the current at
t=0, and the instantaneous power of that resistor at t=0.  And only at
t=0.

When you Alt-left-click on that resistor, the plot window shows the
instantaneous power of R2 not just at t=0, but for all t (time) where
it was simulated.  As you can see, that plot does indeed begin at 0mW
at t=0, and later jumps to 850mW.

Now, what LTspice shows you in the lower left corner, does depend on
the component.  There is a difference between 2-pin and 3-pin
components because 2-pin components have only one current (the current
into and out of the component) but 3-pin devices have 3 unequal
currents.  And there seems to be a difference between transistors with
.MODEL definitions and transistors with .SUBCKT definitions.  I guess
this is where Darlingtons show different results than non-Darlingtons.
This is just the way SPICE works.  That information may not be
available to SPICE, so LTspice can't show you.  But you can get that
information by plotting Power(time).

I hope some of this helps.

Regards,
Andy

Re: .wav files

#90103

Hello Teodor,

Please run the examples you got wit LTspice.

wavein.asc, waveout.asc, ring.wav

C:\Program Files (x86)\LTC\LTspiceIV\examples\Educational?

Best regards,

Helmut

Re: Sub circuit heat dissipation not showing

#90127

Hello Brad,

> What I am missing something?

Ctrl left mouse click on the plot formula in the waveform viewer.?

LTspice will then show a small window with the average power.

Best regards,

Helmut

PS: Second attempt to write an answer.?

I have again problems with delayed or not delivered messages.

.wav files

#90102

Hello,

I do have a problem in using a .wav file as a input voltage source.

I have followed the instructions of Spice Guru Simon Bramble in this video:


			Simon Bramble - Field Applications Engineer This video highlights how to import and export WAV audio files in LTspice as well as how to read a list of ...
				Preview by Yahoo

but it doesn't work. When I'm running the simulation I get this error: "Wavefile: Missing node(s)"

What could be wrong?

My two SPICE directives look like this:

.tran 2

wavefile=Hello.wav

...and for the voltage source I have entered "wavefile=Hello.wav" as a value.

Thanks in advance for your support!

Regards

Teodor

Re: Sub circuit heat dissipation not showing

#90124

Nit:

? ?"there is **no such thing** as 'RMS power'."

Well, there is, but you wouldn't find it a useful thing to compute.? As you said, it has no physical significance.? So nobody ever calculates RMS power.

Andy

?

Re: Sub circuit heat dissipation not showing

#90140

Hello Brad,

> What I am missing something?

Ctrl left mouse click on the power formula in the waveform window. Then you will get a single number which is the average power.

Best regards,

Helmut

Re: Sub circuit heat dissipation not showing

John Woodgate

#90101

Not an answer to your question, but there is **no such thing** as 'RMS power'. The product of RMS voltage and RMS current with zero phase difference is 'average power'.

For pedants, one can calculate a quantity by applying the calculus for RMS to instantaneous power, but it has no physical significance.

With best wishes DESIGN IT IN! OOO – Own Opinions Only
 <> www.jmwa.demon.co.uk J M Woodgate and Associates Rayleigh England

Sylvae in aeternum manent.

From: LTspice@... [mailto:LTspice@...]
Sent: Thursday, August 4, 2016 3:47 AM
To: LTspice@...
Subject: [LTspice] Re: Sub circuit heat dissipation not showing

Helmut,

I know you said "All the Darlington transistors in my examples correctly plot power" But that's not my issue.

I can see the plot/s but I was thinking I would see "dissipation" in watts as with BJT transistors or other non-sub circuits.

I did download and run the TIP142 sub circuit files. I get the same thing. "Left click to plot Q10 dissipation. V(c10)*Ix(Q10:C)+V(b10)*Ix(Q10:B)". But as I think I said earlier I was expecting "dissipation = XXXX" at the end of the formula.

Interestingly, I noticed that R2 said "dissipation = 0" but when I plot it I see about 850 mW for about 50 us at 50% duty cycle. So wouldn't there be some power dissipation here??

Although the plot (for dissipation) is very useful I guess I was thinking I would see a single value for power dissipation (probably RMS power) for that darlington or even R2.

What I am missing something??

Remember I am a beginner and Thanks,
Brad

---In LTspice@... <mailto:LTspice@...> , <helmutsennewald@... <mailto:helmutsennewald@...> > wrote :
Hello,

The power dissipation of the TIP142 from our Files section will be correctly displayed.
TIP_142_test.zip
 ahoo.com/neo/groups/LTspice/files/%20Lib/ <>

Here are a few more examples. Their power will be displayed too.

All the Darlington transistors in my examples correctly plot power.

In therory there are subcircuits possible where LTspice doesn't plot the power due to special combinations of sources internally connected to the pins of a subcircuit.

You should upload your files for a test.

Best regards,
Helmut

I download and ran the TIP142 sub circuit files. I get the same thing. "Left click to plot Q10 dissipation. V(c10)*Ix(Q10:C)+V(b10)*Ix(Q10:B)" I can see the plot but I was thinking I would see "dissipation" in watts as with BJT transistors.

Interestingly, I noticed that R2 said "dissipation = 0" but when I plot it I see about 850 mW for about 50 us at 50% duty cycle. So wouldn't there be some power dissipation here??

Although the plot (for dissipation) is very useful I guess I was thinking I would see a single value for power dissipation (probably RMS power) for that darlington or even R2.

What I am missing something??

Thanks,
Brad

---In LTspice@... <mailto:LTspice@...> , <helmutsennewald@... <mailto:helmutsennewald@...> > wrote :
Hello,

The power dissipation of the TIP142 from our Files section will be correctly displayed.
TIP_142_test.zip

Here are a few more examples. Their power will be displayed too.

All the Darlington transistors in my examples correctly plot power.

In therory there are subcircuits possible where LTspice doesn't plot the power due to special combinations of sources internally connected to the pins of a subcircuit.

You should upload your files for a test.

Best regards,
Helmut

Re: "4 GROUP.zip" upload

#90236

Thanks Andy, I'm still working on fully understanding your post.

Thanks?Bordodynov, I added your 2 model.s ?The BS250P returned and error. "Error on line 602 : .model bs250p vdmos pchan rg=160 vto=-3.193 rs=2.041 rd=0.697 is=2e-13 kp=0.277 cjo=105p pb=1 lambda=1.2e-2 rb=0.309 rds=1.2e8 cgdmax=57p cgdmin=5p cgs=47p tt=86.56n bv=45 ibv=10u

* Unrecognized parameter "pb" -- ignored" so I deleted the PB component.?

Andy, I understand the possibility of sharing a file that has my custom components with others, as is the case where I used the 2n7000 instead of the 2n7002, they both have the same parameters in my CMP file, so I thinking that all my custom component should start with the letter K or J just to remind me to include the model or sub file. Is there a "place" that has the definition of all the parameters of components, vto=-3, lambda=1.2e and such?

Thanks for the help,

Jeff

Re: Need help to design a transimpedance amplifier

#90099

开云体育

Hi there,

Please, Please see an Idea I have posted in the Temp Folders of this group. (Photo Amplifier15.asc)

Best regards,

Michael P Kiwanuka

To: LTspice@...
From: LTspice@...
Date: Fri, 5 Aug 2016 09:10:31 +0200
Subject: Re: [LTspice] Re: Need help to design a transimpedance amplifier

I tried to answer a couple of days ago, but it didn't come through, so I'll write it again:
The noise you observe compes from the fact that you have these big 100k resistors in the non-inverting inputs. The OPA2846 has a very high NOISE CURRENT; it is designed for low-impedance sources. There should be no resistor in the non-inverting inputs, or very low (similar to the APD's equivalent resistance); if used, this resistor should be bypassed by a capacitor, for near-zero impedance within the circuit's BW. That's VLN 101.

Le 04/08/2016 à 09:31, t.obulesu@... [LTspice] a écrit?:

?
Let me say why am looking for new design..
We are currently using the receiver module which has three stages:
1. Trans Impedance stage
2. High Pass filter (HPF) stage
3. Unity gain amplifier (just for inverting the output of the HPF)

Well...we used LM2662 as a -5V supply..
Here on we could see the hell noise below 100kHz..
I couldn't get rid of this noise by using bypass caps..but I could just reduced it..
Yet there is a lot of noise all across the circuit ranging from few kHz to hundreds of MHz...

are the links where I have uploaded couple of documents..

I really don't know what sort of noise it is and from where it is coming...

L'absence de virus dans ce courrier électronique a été vérifiée par le logiciel antivirus Avast.

Re: Henry's current transformer problem

#90108

From the available data we have not seen Br depending temperature change from 25° C to 100° C.

Bordodynov.

05.08.2016, 15:56, "hkafeman@... [LTspice]" <ltspice@...>:

Show quoted text

Borodoynov

Thank you that looks like a good typical material to use.

My understanding is then that given that I am operating at only 50Hz with just some high frequency transients, that any core losses will be insignificant.

Then I can model in LTSpice the effects of ambient temperature using e.g.:

Hc = 22 at 25C decreasing by 0.12 % per C
Bs = 490m at 25C decreasing by 0.27 % per C
Br = 100m at 25C - Does this have a temperature coefficient?

Thanks and Regards
Henry Kafeman

Re: Henry's current transformer problem

[email protected]

#90097

Borodoynov

Thank you that looks like a good typical material to use.

My understanding is then that given that I am operating at only 50Hz with just some high frequency transients, that any core losses will be insignificant.

Then I can model in LTSpice the effects of ambient temperature using e.g.:

Hc = 22 at 25C decreasing by 0.12 % per C
Bs = 490m at 25C decreasing by 0.27 % per C
Br = 100m at 25C - Does this have a temperature coefficient?

Thanks and Regards
Henry Kafeman

Re: Henry's current transformer problem

#90096

Hello Henry Kafeman.
See material N41
BS (25 °C)=490mT
BS (100 °C)=390mT
Hc (25 °C)=22A/m
Hc (100 °C)=20A/m
Br=0.1T

Power
Transformer (low loss)

f<100 kHz

N27 (?i = 2000 ) low cost, hi-power
N41 (?i = 2800 ) current transformer
N51 (?i = 3000 ) loss min. @ 40°C

Bordodynov.

05.08.2016, 14:27, "HKafeman hkafeman@... [LTspice]" <ltspice@...>:

Show quoted text

analogspiceman and Andy

Thank you for your replies.

I appreciate that there are many different Ferrite materials. I do not know which specific material my CT is made of, so am looking to model a typical material.

The typical Hc value for Ferrites I found was 0.2 Oersteds.

I now realise that LTSpice uses Hc in A/m and "0.2 Oersteds = 15.9 A/m". So I need to use Hc in LTSpice of 15.9.

Sorry for the confusion about the path length (for some strange reason I was getting confused with area!) - of course it is Pi * d for the CT (with outer and inner diameters of 28.5 and 17.0mm). So in my case is 71.47mm using the average diameter, so Lm is 71.47m.

Similarly the Area for my CT (width 18mm), A is 103.5u.

Can you help me out with one other aspect of my CT please?

The manufacturer states it is rated at 0.01VA. Now I think this is the maximum Voltage * Current through the Burden Resistor.

But how does this relate to the Secondary Coil power dissipation and also dissipation in the Core?

What happens if this value is exceeded? Does it just mean that the Secondary Coil and Core are heated up significantly which affects the linearity, etc.?

Can this affect be modelled?

Thanks and Regards

Henry Kafeman

Re: Henry's current transformer problem

HKafeman

#90095

analogspiceman and Andy

Thank you for your replies.

I appreciate that there are many different Ferrite materials. I do not know which specific material my CT is made of, so am looking to model a typical material.

The typical Hc value for Ferrites I found was 0.2 Oersteds.

I now realise that LTSpice uses Hc in A/m and "0.2 Oersteds = 15.9 A/m". So I need to use Hc in LTSpice of 15.9.

Sorry for the confusion about the path length (for some strange reason I was getting confused with area!) - of course it is Pi * d for the CT (with outer and inner diameters of 28.5 and 17.0mm). So in my case is 71.47mm using the average diameter, so Lm is 71.47m.

Similarly the Area for my CT (width 18mm), A is 103.5u.

?

Can you help me out with one other aspect of my CT please?

The manufacturer states it is rated at 0.01VA. Now I think this is the maximum Voltage * Current through the Burden Resistor.

But how does this relate to the Secondary Coil power dissipation and also dissipation in the Core?

What happens if this value is exceeded? Does it just mean that the Secondary Coil and Core are heated up significantly which affects the linearity, etc.?

Can this affect be modelled?

Thanks and Regards

Henry Kafeman

Re: Need help to design a transimpedance amplifier

[email protected]

#90093

Thanks for your response Jerry Lee Marcel..
But...I could see this noise everywhere in the circuit..
I mean power supply as well...

Re: Need help to design a transimpedance amplifier

#90110

I design a lot of TIA type of amp. I don't know what kind of speed you are looking for. But your requirement is very easy, the lowest is 200nA. Any opamp with bias current of less than 10nA will work good enough.

I use LTC6268 for my design. It is likely to be way over kill for you. Check out other opamp from LT. A tip for you, I tested out a lot of opamps from Ti and Maxim. Most don't quite meet the spec on the noise even the spec say so. LT6268 really produce the result according to the spec.

Contact Glen Brisebois in LT linear opamp application group. He is very knowledgeable and helpful. I visited him in the head quarters once and he showed me a lot of tricks.

Re: Need help to design a transimpedance amplifier

#90090

开云体育

I tried to answer a couple of days ago, but it didn't come through, so I'll write it again:

The noise you observe compes from the fact that you have these big 100k resistors in the non-inverting inputs. The OPA2846 has a very high NOISE CURRENT; it is designed for low-impedance sources. There should be no resistor in the non-inverting inputs, or very low (similar to the APD's equivalent resistance); if used, this resistor should be bypassed by a capacitor, for near-zero impedance within the circuit's BW. That's VLN 101.

Le 04/08/2016 à 09:31, t.obulesu@... [LTspice] a écrit?:

?

Let me say why am looking for new design..
We are currently using the receiver module which has three stages:
1. Trans Impedance stage
2. High Pass filter (HPF) stage
3. Unity gain amplifier (just for inverting the output of the HPF)

Well...we used LM2662 as a -5V supply..
Here on we could see the hell noise below 100kHz..
I couldn't get rid of this noise by using bypass caps..but I could just reduced it..
Yet there is a lot of noise all across the circuit ranging from few kHz to hundreds of MHz...

are the links where I have uploaded couple of documents..

I really don't know what sort of noise it is and from where it is coming...

L'absence de virus dans ce courrier électronique a été vérifiée par le logiciel antivirus Avast.

Re: "4 GROUP.zip" upload

#90089

I am sorry.
.MODEL BS250P ....

Bordodynov. 

05.08.2016, 09:35, "Александр Бордодынов BordodunovAlex@... [LTspice]" <ltspice@...>:

Show quoted text

Hi.
.model BS170 VDMOS VTO=1.824 RG=270 RS=1.572 RD=1.436 RB=.768 KP=.1233 Cgdmax=20p Cgdmin=3p CGS=28p Cjo=35p Rds=1.2E8 IS=5p Bv=60 Ibv=10u Tt=161.6n
.MODEL BS250 VDMOS pchan Rg=160 VTO=-3.193 RS=2.041 RD=0.697 IS=2E-13 KP=0.277 Cjo=105p PB=1 LAMBDA=1.2E-2 RB=0.309 Rds=1.2E8 Cgdmax=57p Cgdmin=5p CGS=47p TT=86.56n BV=45 IBV=10u

Bordodynov.

05.08.2016, 08:56, "Andy ai.egrps@... [LTspice]" <ltspice@...>:
Jeff asked:

? ?"Is there an easy or a standard way to make a model for these transistors that can be included in LIB/cmp/standard.mos?"

For the?BS250P and BS170?transistor models you used, no, there isn't.? Those particular models are .SUBCKTs.? You can't have a subcircuit model in the "standard.mos" file.? That file is only for transistor models that use just the .MODEL syntax; it's not for subcircuits.

But aside from that .. this is a touchy question.

Aside from MS-Windows, there is nothing stopping you from editing your lib&#92;cmp&#92;standard.mos file, and adding your own MOSFET models to it if they are .MODEL models.? In fact, the LTspice Help pages even recommend it (Help: F.A.Q. -> MOSFET Models), so Mike Engelhardt thought it was OK.? Many people here in this group recommend against editing that file, but you can.

Windows might require you to be the Administrator, when you edit the file.

Of the lib&#92;cmp&#92;standard.* files, these ones are text files and could be edited directly:

standard.bjt
standard.dio
standard.jft
standard.mos

(The others are binary.)

The format is ordinary SPICE Netlist format, and should be just a .MODEL statement for each diode or transistor.? Obviously, device names must not clash, and standard SPICE rules apply about continuation lines.? Also, use only a decent text editor that does not add stray binary bytes here and there.? Notepad is best avoided.

Indeed there are enhanced versions of the standard.* files with many more transistors in them, which people have contributed to the LTspice user community.? They can be found in a few places in this group's Files area, and on the LTwiki website (ltwiki.org).

One of the problems with editing your standard.mos file (rather than pasting .MODEL statements on your schematic or having them in a separate file), is that you may forget that other LTspice users don't have those same transistors in their LTspice installation.? Then when you send them your schematic that uses one of those transistors, the schematic cannot be run.? Having those .MODEL statements separate, makes it more likely for you to send the .MODELs along with your schematic.

Regards,
Andy

Re: "4 GROUP.zip" upload

#90088

Hi.
.model BS170 VDMOS VTO=1.824 RG=270 RS=1.572 RD=1.436 RB=.768 KP=.1233 Cgdmax=20p Cgdmin=3p CGS=28p Cjo=35p Rds=1.2E8 IS=5p Bv=60 Ibv=10u Tt=161.6n
.MODEL BS250 VDMOS pchan Rg=160 VTO=-3.193 RS=2.041 RD=0.697 IS=2E-13 KP=0.277 Cjo=105p PB=1 LAMBDA=1.2E-2 RB=0.309 Rds=1.2E8 Cgdmax=57p Cgdmin=5p CGS=47p TT=86.56n BV=45 IBV=10u

Bordodynov.

05.08.2016, 08:56, "Andy ai.egrps@... [LTspice]" <ltspice@...>:

Show quoted text

Jeff asked:

? ?"Is there an easy or a standard way to make a model for these transistors that can be included in LIB/cmp/standard.mos?"

For the?BS250P and BS170?transistor models you used, no, there isn't.? Those particular models are .SUBCKTs.? You can't have a subcircuit model in the "standard.mos" file.? That file is only for transistor models that use just the .MODEL syntax; it's not for subcircuits.

But aside from that .. this is a touchy question.

Aside from MS-Windows, there is nothing stopping you from editing your lib&#92;cmp&#92;standard.mos file, and adding your own MOSFET models to it if they are .MODEL models.? In fact, the LTspice Help pages even recommend it (Help: F.A.Q. -> MOSFET Models), so Mike Engelhardt thought it was OK.? Many people here in this group recommend against editing that file, but you can.

Windows might require you to be the Administrator, when you edit the file.

Of the lib&#92;cmp&#92;standard.* files, these ones are text files and could be edited directly:

standard.bjt
standard.dio
standard.jft
standard.mos

(The others are binary.)

The format is ordinary SPICE Netlist format, and should be just a .MODEL statement for each diode or transistor.? Obviously, device names must not clash, and standard SPICE rules apply about continuation lines.? Also, use only a decent text editor that does not add stray binary bytes here and there.? Notepad is best avoided.

Indeed there are enhanced versions of the standard.* files with many more transistors in them, which people have contributed to the LTspice user community.? They can be found in a few places in this group's Files area, and on the LTwiki website (ltwiki.org).

One of the problems with editing your standard.mos file (rather than pasting .MODEL statements on your schematic or having them in a separate file), is that you may forget that other LTspice users don't have those same transistors in their LTspice installation.? Then when you send them your schematic that uses one of those transistors, the schematic cannot be run.? Having those .MODEL statements separate, makes it more likely for you to send the .MODELs along with your schematic.

Regards,
Andy

Re: PWL TRIGGER syntax

#90087

> does somebody have problem with this syntax? PWL (0 0 1m 1 2m 1 3m 0) TRIGGER V(n003)>1
> the error msg I receieve is Unknown parameter "trigger"

Without knowing what you have, if you're using the "trigger" keyword with current sources, it doesn't work, only for voltage sources.

Vlad
______________________
-- holding, among others:
a universal analog/digital filter, block-level models
for power electronics (and not only), math blocks
with a more stream-lined approach, some digital
ADC, DAC, (synchronous-)counter, JKflop, etc.

Re: BS250 & BS170 SIM

#90084

Jeff wrote:

? ?"they look like they should work, but the don't, how can I add them to my CMP folder, that is what is the correct model layout."

I just noticed you sent this question two days ago.? It finally went through Yahoo's servers!? It got held up that long.

I think you already have the answer to this question.

Andy