Re: Simulating Dirty Battery Contact
--- In LTspice@..., "octavefiddler" <ruhroh88@...> wrote:
The R-value by function is new to me, having never noticed it before.
I always thought the only way to make a resistance which changes during the sim, is by the MySwitch example, which is rather binary by nature.
The R= function doesn't seem to work for inductors,
which I guess explains the long efforts to implement non-linear inductance.
Octave
Octave, LTspice has 2 noninear inductance models. For one of them you need to provide an equation for the flux, and for the other you need to give core parameters and the gap. LTspice also can handle nonlinear caps. See the help file for more information on these. Rick
|
Re: Simulating Dirty Battery Contact
Dear Sir;
I often use LTspice as a way to communicate circuit concepts to my distant colleagues. Expressing variable resistances as R= some-function, will greatly comfort those folks who have limited ability to internalize novel (to them) Spice constructs ( such as B-sources) simultaneously to comprehend the larger point I am trying to make with my lecture.
Looking back at the NiMH model, I see he uses the "R=" construction,
and the table is accessed according to a voltage V(1,K) ;
I guess the simple beauty of "R=" was not readily obvious to me when I 'studied' that model.
Regarding 'normally' , if you ever met me, you would realize that is not germanium to me.
Actually battery 'esr' is probably a fairly ubiquitous issue, and variable contact resistance is another such issue. So, I think it is valuable to convey this R= thing more broadly. I still can't find it in the help pages.
Best,
Octave
toggle quoted message
Show quoted text
--- In LTspice@..., "Helmut" <helmutsennewald@...> wrote:
Hello Octave,
Normally one doesn't need this function. If you look in the
SPICE error log file, you will see that it's replaced by a
B-source. So it's not an extra R-model. It's simply a little
bit comfort in some cases.
Best regards,
Helmut
--- In LTspice@..., "octavefiddler" <ruhroh88@> wrote:
The R-value by function is new to me, having never noticed it before.
I always thought the only way to make a resistance which changes during the sim, is by the MySwitch example, which is rather binary by nature.
The R= function doesn't seem to work for inductors,
which I guess explains the long efforts to implement non-linear inductance.
I appreciate you bringing this to my attention,
without regard to it being long-established.
From whence might I have learned of this Capability?
I've never seen anyone do this,
even though I thought I was studying the guru's...
My world has many variable resistances in it, and they are not trimpots.
I will try to explore the limits of this (new-to-me) functionality, but other clues are welcome.
Am I the only person who didn't know this?
Thanks again,
Octave
--- In LTspice@..., "Helmut" <helmutsennewald@> wrote:
Hello Octave,
The R-function R=any_forumala is since many years available
in LTspice.
Please be aware that such pseudo-resistors have no noise in
a .NOISE-analysis. It's also independent of any AC-voltage
in the .AC-analysis. The formula is then only used at the
beginning of a simulation to get a DC operating point.
Best regards,
Helmut
--- In LTspice@..., "octavefiddler" <ruhroh88@> wrote:
Helmut;
This is a wonderful example, thanks.
I'm a bit surprised that it is OK to make a component parameter to be a
function of a node voltage.
At minimum I would have assumed a need for {curly braces} .
But no, you just made a voltage controlled variable resistor.
Is this a new capability for LTspice?
What are the limits on how I can make a device parameter a continuously variable function of a ~dynamic voltage or current?
I thought that this sentence from the help file meant no intra-sim dynamic values;
"All parameter substitution evaluation is done before the simulation begins"
Thanks for all that you do.
Regards,
Octave
--- In LTspice@..., "Helmut" <helmutsennewald@> wrote:
--- In LTspice@..., "sckottyj" wrote:
I'm trying to simulate a dirty or intermittent battery contact with
either a variable resistor or the voltage controlled switch.
Unfortunately, it only seems to work with resistive loads. I get the
same results, so I will only explain the variable resistor technique.
My virtual battery is setup as a voltage source (DC value = 3.3) and is
connected to ground via an inductor and resistor (part of our
circuitry).
The positive terminal of the battery is connected to a resistor with
R=V(VAR). I've setup a 2nd voltage source with a net label VAR on the
positive net. The 2nd voltage source is grounded and is configured with
a pulse function.
Now, when I load the variable resistor output (the other terminal which
is not connected to the battery) with a resistor to ground, I observe
the switched voltage as anticipated. But if I load the variable
resistor with a capacitor or any other circuit to ground, all I see is
the DC battery voltage on the output of the variable resistor?
Anyone know why?
Hello "sckottyj",
I can't reproduce your problem.
Please try may uploaded example and change it to your case.
Files > Temp > R_time.asc
Best regards,
Helmut
|
Re: Simulating Dirty Battery Contact
Hello Octave,
Normally one doesn't need this function. If you look in the
SPICE error log file, you will see that it's replaced by a
B-source. So it's not an extra R-model. It's simply a little
bit comfort in some cases.
Best regards,
Helmut
toggle quoted message
Show quoted text
--- In LTspice@..., "octavefiddler" <ruhroh88@...> wrote:
The R-value by function is new to me, having never noticed it before.
I always thought the only way to make a resistance which changes during the sim, is by the MySwitch example, which is rather binary by nature.
The R= function doesn't seem to work for inductors,
which I guess explains the long efforts to implement non-linear inductance.
I appreciate you bringing this to my attention,
without regard to it being long-established.
From whence might I have learned of this Capability?
I've never seen anyone do this,
even though I thought I was studying the guru's...
My world has many variable resistances in it, and they are not trimpots.
I will try to explore the limits of this (new-to-me) functionality, but other clues are welcome.
Am I the only person who didn't know this?
Thanks again,
Octave
--- In LTspice@..., "Helmut" <helmutsennewald@> wrote:
Hello Octave,
The R-function R=any_forumala is since many years available
in LTspice.
Please be aware that such pseudo-resistors have no noise in
a .NOISE-analysis. It's also independent of any AC-voltage
in the .AC-analysis. The formula is then only used at the
beginning of a simulation to get a DC operating point.
Best regards,
Helmut
--- In LTspice@..., "octavefiddler" <ruhroh88@> wrote:
Helmut;
This is a wonderful example, thanks.
I'm a bit surprised that it is OK to make a component parameter to be a
function of a node voltage.
At minimum I would have assumed a need for {curly braces} .
But no, you just made a voltage controlled variable resistor.
Is this a new capability for LTspice?
What are the limits on how I can make a device parameter a continuously variable function of a ~dynamic voltage or current?
I thought that this sentence from the help file meant no intra-sim dynamic values;
"All parameter substitution evaluation is done before the simulation begins"
Thanks for all that you do.
Regards,
Octave
--- In LTspice@..., "Helmut" <helmutsennewald@> wrote:
--- In LTspice@..., "sckottyj" wrote:
I'm trying to simulate a dirty or intermittent battery contact with
either a variable resistor or the voltage controlled switch.
Unfortunately, it only seems to work with resistive loads. I get the
same results, so I will only explain the variable resistor technique.
My virtual battery is setup as a voltage source (DC value = 3.3) and is
connected to ground via an inductor and resistor (part of our
circuitry).
The positive terminal of the battery is connected to a resistor with
R=V(VAR). I've setup a 2nd voltage source with a net label VAR on the
positive net. The 2nd voltage source is grounded and is configured with
a pulse function.
Now, when I load the variable resistor output (the other terminal which
is not connected to the battery) with a resistor to ground, I observe
the switched voltage as anticipated. But if I load the variable
resistor with a capacitor or any other circuit to ground, all I see is
the DC battery voltage on the output of the variable resistor?
Anyone know why?
Hello "sckottyj",
I can't reproduce your problem.
Please try may uploaded example and change it to your case.
Files > Temp > R_time.asc
Best regards,
Helmut
|
Re: Simulating Dirty Battery Contact
The R-value by function is new to me, having never noticed it before.
I always thought the only way to make a resistance which changes during the sim, is by the MySwitch example, which is rather binary by nature.
The R= function doesn't seem to work for inductors,
which I guess explains the long efforts to implement non-linear inductance.
I appreciate you bringing this to my attention,
without regard to it being long-established.
From whence might I have learned of this Capability?
I've never seen anyone do this,
even though I thought I was studying the guru's...
My world has many variable resistances in it, and they are not trimpots.
I will try to explore the limits of this (new-to-me) functionality, but other clues are welcome.
Am I the only person who didn't know this?
Thanks again,
Octave
toggle quoted message
Show quoted text
--- In LTspice@..., "Helmut" <helmutsennewald@...> wrote:
Hello Octave,
The R-function R=any_forumala is since many years available
in LTspice.
Please be aware that such pseudo-resistors have no noise in
a .NOISE-analysis. It's also independent of any AC-voltage
in the .AC-analysis. The formula is then only used at the
beginning of a simulation to get a DC operating point.
Best regards,
Helmut
--- In LTspice@..., "octavefiddler" <ruhroh88@> wrote:
Helmut;
This is a wonderful example, thanks.
I'm a bit surprised that it is OK to make a component parameter to be a
function of a node voltage.
At minimum I would have assumed a need for {curly braces} .
But no, you just made a voltage controlled variable resistor.
Is this a new capability for LTspice?
What are the limits on how I can make a device parameter a continuously variable function of a ~dynamic voltage or current?
I thought that this sentence from the help file meant no intra-sim dynamic values;
"All parameter substitution evaluation is done before the simulation begins"
Thanks for all that you do.
Regards,
Octave
--- In LTspice@..., "Helmut" <helmutsennewald@> wrote:
--- In LTspice@..., "sckottyj" wrote:
I'm trying to simulate a dirty or intermittent battery contact with
either a variable resistor or the voltage controlled switch.
Unfortunately, it only seems to work with resistive loads. I get the
same results, so I will only explain the variable resistor technique.
My virtual battery is setup as a voltage source (DC value = 3.3) and is
connected to ground via an inductor and resistor (part of our
circuitry).
The positive terminal of the battery is connected to a resistor with
R=V(VAR). I've setup a 2nd voltage source with a net label VAR on the
positive net. The 2nd voltage source is grounded and is configured with
a pulse function.
Now, when I load the variable resistor output (the other terminal which
is not connected to the battery) with a resistor to ground, I observe
the switched voltage as anticipated. But if I load the variable
resistor with a capacitor or any other circuit to ground, all I see is
the DC battery voltage on the output of the variable resistor?
Anyone know why?
Hello "sckottyj",
I can't reproduce your problem.
Please try may uploaded example and change it to your case.
Files > Temp > R_time.asc
Best regards,
Helmut
|
Re: Simulating Dirty Battery Contact
I thought that this sentence from the help file meant no intra-sim dynamic values;
"All parameter substitution evaluation is done before the simulation begins" I think that limitation applies specifically to the .PARAM statement.
|
Hey folks:
I am looking for documentation on the standard.___ files. Some of
these files are in a binary format, and I would like to create a few
scripts to put our qualified components into these files. The ability
to script this would be a great asset, and a time saver.
I am specifically looking for documentation on:
standard.bead
standard.cap
standard.ind
standard.res
Thank you for your time,
Tim Jameson
|
Re: Simulating Dirty Battery Contact
Hello Octave,
The R-function R=any_forumala is since many years available
in LTspice.
Please be aware that such pseudo-resistors have no noise in
a .NOISE-analysis. It's also independent of any AC-voltage
in the .AC-analysis. The formula is then only used at the
beginning of a simulation to get a DC operating point.
Best regards,
Helmut
toggle quoted message
Show quoted text
--- In LTspice@..., "octavefiddler" <ruhroh88@...> wrote:
Helmut;
This is a wonderful example, thanks.
I'm a bit surprised that it is OK to make a component parameter to be a
function of a node voltage.
At minimum I would have assumed a need for {curly braces} .
But no, you just made a voltage controlled variable resistor.
Is this a new capability for LTspice?
What are the limits on how I can make a device parameter a continuously variable function of a ~dynamic voltage or current?
I thought that this sentence from the help file meant no intra-sim dynamic values;
"All parameter substitution evaluation is done before the simulation begins"
Thanks for all that you do.
Regards,
Octave
--- In LTspice@..., "Helmut" <helmutsennewald@> wrote:
--- In LTspice@..., "sckottyj" wrote:
I'm trying to simulate a dirty or intermittent battery contact with
either a variable resistor or the voltage controlled switch.
Unfortunately, it only seems to work with resistive loads. I get the
same results, so I will only explain the variable resistor technique.
My virtual battery is setup as a voltage source (DC value = 3.3) and is
connected to ground via an inductor and resistor (part of our
circuitry).
The positive terminal of the battery is connected to a resistor with
R=V(VAR). I've setup a 2nd voltage source with a net label VAR on the
positive net. The 2nd voltage source is grounded and is configured with
a pulse function.
Now, when I load the variable resistor output (the other terminal which
is not connected to the battery) with a resistor to ground, I observe
the switched voltage as anticipated. But if I load the variable
resistor with a capacitor or any other circuit to ground, all I see is
the DC battery voltage on the output of the variable resistor?
Anyone know why?
Hello "sckottyj",
I can't reproduce your problem.
Please try may uploaded example and change it to your case.
Files > Temp > R_time.asc
Best regards,
Helmut
|
--- In LTspice@..., sourav chatterjee <sourav_ece24@...> wrote:
Hi,? I am doing transcient Analysis of ?a netlist file in LTSpice as well as in HSPICE. But I am getting different ?waveform.I want to know what is the reason for this difference.. I am attaching Spice netlist for your kind persusal.
With regards,Souarv
Hello Sourav, I run your files and it looks OK. Could you please upload a screenshot with the result of HSPICE. You could switch off data compression to be sure that the calculated results will not be reduced to save disk storage. .options plotwinsize=0 You can additionally reduce the maximum time step. .tran 0 200p 0 0.01p Best regards, Helmut
|
Re: Simulating Dirty Battery Contact
Helmut;
This is a wonderful example, thanks.
I'm a bit surprised that it is OK to make a component parameter to be a
function of a node voltage.
At minimum I would have assumed a need for {curly braces} .
But no, you just made a voltage controlled variable resistor.
Is this a new capability for LTspice?
What are the limits on how I can make a device parameter a continuously variable function of a ~dynamic voltage or current?
I thought that this sentence from the help file meant no intra-sim dynamic values;
"All parameter substitution evaluation is done before the simulation begins"
Thanks for all that you do.
Regards,
Octave
toggle quoted message
Show quoted text
--- In LTspice@..., "Helmut" <helmutsennewald@...> wrote:
--- In LTspice@..., "sckottyj" wrote:
I'm trying to simulate a dirty or intermittent battery contact with
either a variable resistor or the voltage controlled switch.
Unfortunately, it only seems to work with resistive loads. I get the
same results, so I will only explain the variable resistor technique.
My virtual battery is setup as a voltage source (DC value = 3.3) and is
connected to ground via an inductor and resistor (part of our
circuitry).
The positive terminal of the battery is connected to a resistor with
R=V(VAR). I've setup a 2nd voltage source with a net label VAR on the
positive net. The 2nd voltage source is grounded and is configured with
a pulse function.
Now, when I load the variable resistor output (the other terminal which
is not connected to the battery) with a resistor to ground, I observe
the switched voltage as anticipated. But if I load the variable
resistor with a capacitor or any other circuit to ground, all I see is
the DC battery voltage on the output of the variable resistor?
Anyone know why?
Hello "sckottyj",
I can't reproduce your problem.
Please try may uploaded example and change it to your case.
Files > Temp > R_time.asc
Best regards,
Helmut
|
The file, 'basic feedback scheme for OpAmp with R(f)' is too big, That is because you tried to upload .rtf (Rich Text Format) files. The RTF file format is one of the most wasteful ones in terms of file space. Also, RTF is a word processing file format, so I am puzzled why you used that for LTspice schematics. Please don't do that. The preferred file format for LTspice is its native schematic file, normally "something.asc". If you have the schematics saved from LTspice, then find those files and upload them instead. They are about a thousand times smaller (literally) than RTF files. If all you have is a graphic file (say, something.gif or something.jpg), then upload that. If you only have those .rtf files and are using them in Microsoft Word, please save them as Word .doc files, which will be a lot smaller. Please make sure to save them as .doc, NOT as .docx which is Word's newer format and is not compatible with many versions of Word and other word processing programs! Andy
|
Re: Please help with this error..
Thank you folks.. yes it was the second "Mpsa18" on the value line. Just
took it out, and it seems to simulate now. I'll work with it... Thank
You! Thank you!!
A...
toggle quoted message
Show quoted text
--- In LTspice@..., Andy <Andrew.Ingraham@...> wrote:
Error on line 2 : q1 n002 n005 n006 0 mpsa18 mpsa18
Unknown parameter "mpsa18" The problem is the second "mpsa18" on that line.
q1 is the transistor name. n002, n005, n006, and 0 are its four nodes
(you must have used the symbol NPN4 for this transistor, with a
substrate node). The first mpsa18 identifies what kind of transistor
it is, what .MODEL it refers to. So far so good. Anything coming
after that would be interpreted to be an additional parameter for that
element. "mpsa18" is not an allowed parameter.
Did you add something in the Value2 or SpiceLine or SpiceLine2 for
that transistor? (Ctrl-Right Click to get to that menu)
Andy
|
The file, 'basic feedback scheme for OpAmp with R(f)' is too big,
Can any body help me how I can compress it and attach it again.
Michael
|
I have arrived at an LTspice simulation which simulates the gain Vs frequency of the Op Amp with a feedback resistor a function of frequency. I used basic control theory with the help of Helmuts control theory files which can be found in our LTspice Files.
You can find a copy of the display and its cor5esonding schematics in the Temp Files of this group. The files are namely,
1) Op Amp with R(f) feedbck element
2) basic feedbck scheme for Op Amp with R(f).
With reference to the Files
U1 represents a single exponential lag
U2 represents a proportional block
U4 feedback network block of gain Beta
U6 (1/Beta)*Vin
U7 proportional block
V2=V1=Vin
Vxa= output gain with feedback N/W
Vo= output gain with unity feedback scheme for those who use a Nichols chart.
For convinience the time constant is set to unity for the exponential lag.(you can select any to suit your purposes)
You can simulate this work in LTspice IV having copied the relevant files and symbols from Helmut's Control theory files.
The basic underlying idea for the shown scheme is the eqn
Af = (Ao*Beta)/(1 + Ao*Beta)
Michael
|
--- In LTspice@..., sourav chatterjee <sourav_ece24@...> wrote: ... I am attaching Spice netlist for your kind persusal Told every day ... look at the homepage how do share files. Attaching files to messages is not allowed by yahoo. You have to upload files to our temp-directory. <yourfile> As yahoo tells you, attachments are removed [Non-text portions of this message have been removed] hws
|
Hi,? I am doing transcient Analysis of ?a netlist file in LTSpice as well as in HSPICE. But I am getting different ?waveform.I want to know what is the reason for this difference.. I am attaching Spice netlist for your kind persusal.
With regards,Souarv
[Non-text portions of this message have been removed]
|
Hello,
It's easy to probe signals.
Make the waveform window the active window.
Right-mouse-click -> Add Trace
A dialog window will pop-up. Select what you want in this
dialog window.
Best regards,
Helmut
toggle quoted message
Show quoted text
--- In LTspice@..., "sourav" <sourav_ece24@...> wrote:
hi helmut,
Thank you very much for your reply. Now I have a doubt. How I will probe the waveform ?
regards,
Sourav
--- In LTspice@..., "Helmut" <helmutsennewald@> wrote:
--- In LTspice@..., "sourav" <sourav_ece24@> wrote:
Hi,
I am new user to this group. I am using LT spice for one month. I Have a doubt.I have netlist. I want to feed that netlist in the LT-spice. Is there any way to do this?
With regards,
Sourav Chatterjee
Hello Sourav,
I recommend to name the netlist file with the extension .cir .
Then open the netlist with LTspice
File -> Open
A dialog box will pop-up. -> Filetype: Netlist
You could also simply drag this file with Windows Explorer
into LTspice.
Best regards,
Helmut
|
Re: 3rd party transistor model
Hi.
I am sorry.
.Subckt Pmos_simpl D G S kp=5u z=1 A={kp*z} V0=-0.3 b=5
* z=w/l
.Func Vt(x) V0*(1-(abs(x/b))**3) ; F(Vds)
Bids D S i=A*uramp( -(V(G,S)-Vt(v(d,s)) ))*v(D,S) ; < 0
.ends
I place example in /TEMP: Pmos_simpl.asc.
Bordodynov.
|
hi helmut,
Thank you very much for your reply. Now I have a doubt. How I will probe the waveform ?
regards,
Sourav
toggle quoted message
Show quoted text
--- In LTspice@..., "Helmut" <helmutsennewald@...> wrote:
--- In LTspice@..., "sourav" <sourav_ece24@> wrote:
Hi,
I am new user to this group. I am using LT spice for one month. I Have a doubt.I have netlist. I want to feed that netlist in the LT-spice. Is there any way to do this?
With regards,
Sourav Chatterjee
Hello Sourav,
I recommend to name the netlist file with the extension .cir .
Then open the netlist with LTspice
File -> Open
A dialog box will pop-up. -> Filetype: Netlist
You could also simply drag this file with Windows Explorer
into LTspice.
Best regards,
Helmut
|
Re: 3rd party transistor model
Hi.
Example:
.Subckt Pmos_simpl D G S kp=5u z=1 A={kp*z} V0=-0.3 b=5
* z=w/l
Vt(x) V0*(1-(abs(x/b))**3) ; F(Vds)
Bids D S i=A*uramp(-(V(G,S)-Vt(v(d,s)) )*v(D,S) ; < 0
.ends
Bordodynov.
16.04.2013, 10:09, "uppilih" <uppilih@...>:
toggle quoted message
Show quoted text
I have a simple pmos device model that describes Id as a function of Vd and Vg.
IDS = A* (-VG + |B|)* VDS,
where B = Vt = f(Vd)
I don't have any other device specifications. How do I upload this model into LTspice for doing simple logic simulations? I am a high school student. Thanks for any help/suggestions!
|
Re: help with 3rd party model
--- In LTspice@..., "Lance" <lancemcbride@...> wrote:
Can anyone point me to a good tutorial on using 3rd party models in LTSpice. I'm trying to use a power controller from TI. I've tried the LTspice help, created an ".asy" and put a directive in (.INCLUDE ucc28019.lib), but I'm doing something wrong since an error message pops up stating "Missing schematic(s) of the hierarchy: ucc28019".
Thanks for any help.
Hello Lamce, even you have made everything correct in your symbol, it can't be used with LTspice because it's encrypted for PSPICE. These models for the ucc28019 from TI with only work with PSPICE. No other SPICE programs knows the decryption key. .SUBCKT UCC28019 GND ICOMP ISENSE GATE VSENSE VCOMP $CDNENCSTART eee8c5c7a2bc4b01f045f303678664e7916da0bae22e8cb0bba041dd67c 18bd705e89c94b379a904dac3803a9234e68880ca6355b4344fce083935 Best regards, Helmut
|
