Re: AD630 circuit simulation, no line shown
Hello Tob,
Please watch the SPICE-directives in my uploaded file CircuitAD630_1.zip. It contains a few SPICE-directives to achieve convergence. I also removed the absolute paths of the model files in the symbols.?My uploaded file is in the Temp-folder.
By the way there is a nice symbol for the AD630 in the Files section. Best regards, Helmut
|
Re: AD630 circuit simulation, no line shown
Hello Tob,
I tested with the latest LTspiceXVII which has been released today.
Please ad the following SPICE-directives.
.options method=gear
.options gmin=1e-10 abstol=1e-10
.options cshunt=1e-16
.tran 0 0.2 0 1u
By the way there is a nice symbol and example in our Files section.
Best regards,
|
Re: Sub circuit heat dissipation not showing
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: AD630 circuit simulation, no line shown
The purpose of this whole circuit is to test the AD630, so switching it with another op amp would solute my problem :/
Thanks though!
|
Re: AD630 circuit simulation, no line shown
Yes, you are right. It's pretty late here, sorry :/ So my problem is, that I want to simulate the following circuit: [1] Therefore I built up a schematic, which I uploaded in the temp directory as "CircuitAd630": [2] If I hit the simulate button for a transient simulation, there are no lines shown in the diagram, except the ones for the input voltage. Additionally sometimes the simulation needs just a few moments to run and then (without me changing anything) it needs many hours. I tried to locate the error by seperating the two op amps and it looks like the AD630 is the problem here, since the AD8221 works fine, when I simulate it alone by cutting the connections to the righten part of the circuit. Thanks in advance! [1] [2] ?
|
Re: AD630 circuit simulation, no line shown
At 01:51 PM (-0700) 8/3/2016, tob.nagel@... wrote: ---------- Original Message ---------- Hey,
simple task: I want to simulate the circuit in the following picture:
https://s31.postimg.org/cfx03t823/circuit.png
View on s31.postimg.org https://s31.postimg.org/cfx03t823/circuit.png
Preview by Yahoo
Therefore I created this in LTspice:
https://s32.postimg.org/z7tgiq65x/schematic.png
View on s32.postimg.org https://s32.postimg.org/z7tgiq65x/schematic.png
Preview by Yahoo
But when I hit the simulate-button, sometimes it only works with 1ns per second and sometimes it's pretty fast without me changing anything. Additionally there isn't any line in the diagram when i choose the fitting trace. If I remove the right op amplifier (AD630), the rest works fine, so I assume that the problem is here.
I used the netlist provided from AD630 Datasheet and Product Info | Analog Devices
AD630 Datasheet and Product Info | Analog Devices The AD630 is a high precision balanced modulator/demodulatorthat combines a flexible commutating architecture with theaccuracy and temperature stability af
View on www.analog.com
Preview by Yahoo
Can anyone see my mistake? I've spent many hours for searching now...
Thanks! ---------- End of Original Message ---------- Analog Devices models are notorious for causing agony on LTspice. Try AD633_JT.zip on the Device Models & Subcircuits Page of my website. ...Jim Thompson Web Site: <>
|
Re: Sub circuit heat dissipation not showing
Okay Thanks I tried that and still the same thing. Just displays a formula for power dissipation, but I can left click to plot power.?
---In LTspice@..., <analogspiceman@...> wrote : Hello Brad,
Not at my computer right now so I can't check, but maybe you just need to go to the control panel and enable save (subcircuit) currents.
|
Re: high frequency MHz and GHz range BJTtransistor or Mosfet
That ¡°high frequency¡± definition is what is used by the regulators (FCC and their cohorts) to describe transmitted and received signal frequencies. The term is much less precise in actual technical usage. For example: ¡°high frequency amplifier¡± does not characterize it for specific use in the 3-30MHz range, particularly outside of the RF communication arena.
Jim
James Wagner Oregon Research Electronics
toggle quoted message
Show quoted text
? ?"What is your definition of high frequency? For some people, it is 1MHz, for others it might be 10GHz."
By definition, high frequency means 3 MHz to 30 MHz.
Even saying "GHz range" -- does that mean 1 GHz, or 700 GHz?
You gotta love those vague questions....
Andy
?
|
llgveka?wrote:
? ?"I want to understand the operation of a switch made up of a P_MOS and a N_MOS in parallels"
You can read about it here:
I looked for the same page in French, but apparently there is not one.? I am sure the information must be available in all languages, but the name might be different in French.
? ?"and how to assemble them to convert an analogical signal into a numerical signal."
I don't know what that means.? I don't think you can combine only switches to make an Analog-to-Digital (A/D) converter.? I think you need to use other kinds of circuits to do that.
If you need help to understand PMOS and NMOS transistors in a transmission gate switch, then you might not understand how to make an A/D converter yet. ? Keep studying!
Andy
|
Re: AD630 circuit simulation, no line shown
|
LT1171 model and synchronization function
Hi,
Is anyone experienced with the LT1171 and LTSpice.
Is the synchronization function implemented in the model?
I am trying to make a negative buck regulator based on the circuit in the datasheet, but with external clock synchronization (also based on the LT1171 datasheet, page 11). I put my circuit in the Files->Temp folder as Neg Buck 20160803.ZIP. I don't see the switching current synchronizing with my low pulses on the VC pin.
I also tried adding synchronization to the postive boost circuit provided in the LTSpice jigs folder, and got similar results.
Thanks
Matt
|
Re: high frequency MHz and GHz range BJTtransistor or Mosfet
? ?"What is your definition of high frequency? For some people, it is 1MHz, for others it might be 10GHz."
By definition, high frequency means 3 MHz to 30 MHz.
Even saying "GHz range" -- does that mean 1 GHz, or 700 GHz?
You gotta love those vague questions....
Andy
?
|
Re: AD630 circuit simulation, no line shown
tob.nagel?wrote:
? ?"simple task: I want to simulate the circuit in the following picture:"
Please don't send links to off-site file storage areas.
Some of them are like computer viruses.? They take forever to load, and some of those sites start downloading crap to your computer without you clicking anything.? Some of them have so many links to places that actually have computer viruses, that they are dangerous places to go to even if you try to be careful.
Even when those sites are not unsafe, there is no need to direct us to off-site storage areas.
This group you are in has a File storage and a Photo storage area.? Use them.
? ?"Therefore I created this in LTspice:"
Never send photos of your LTspice schematics!? It is not useful when someone does that.
UPLOAD your schematic (the .ASC file, and all models and other things it depends on) to the group's Temp folder:
When you are inconsiderate enough to upload just a photograph or screen capture of your LTspice schematic, you force all of us to re-enter your schematic all over again.? You also deny us from knowing what attributes are attached to your components.? That's why this isn't helpful.
Please, go back and READ and RE-READ the email you received when you joined the group.? Also read the main webpage for the group.? Then try to follow the instructions contained in them.
Andy
|
AD630 circuit simulation, no line shown
Hey, simple task: I want to simulate the circuit in the following picture: https://s31.postimg.org/cfx03t823/circuit.pngTherefore I created this in LTspice: https://s32.postimg.org/z7tgiq65x/schematic.png ? But when I hit the simulate-button, sometimes it only works with 1ns per second and sometimes it's pretty fast without me changing anything. Additionally there isn't any line in the diagram when i choose the fitting trace. If I remove the right op amplifier (AD630), the rest works fine, so I assume that the problem is here. I used the netlist provided from | | | | The AD630 is a high precision balanced modulator/demodulatorthat combines a flexible commutating architecture with theaccuracy and temperature stability af | | | | Preview by Yahoo | | | ?
Can anyone see my mistake? I've spent many hours for searching now...
Thanks!
|
Re: high frequency MHz and GHz range BJTtransistor or Mosfet
Try a 2N918. Small signal, but I think it is in the built-in LTspice library.
Jim
James Wagner Oregon Research Electronics
toggle quoted message
Show quoted text
Shikha wrote:
"Can any one suggest me high frequency BJT Transistor or MOSFET available for working with LTspice."
What is your definition of high frequency? For some people, it is 1MHz, for others it might be 10GHz.
To make it a bit easier for you, the following few suggestions have manufacturer-supplied SPICE models: BF998 (N-ch DG MOS) BFR92AW (NPN BJT)
BFT92W (PNP BJT)
Your best bets for SPICE models for RF transistors are the NXP or Infineon websites.?Also, try the group's Files section. I suspect from your question, you haven't actually looked very hard yet.
Regards, Tony
|
Re: high frequency MHz and GHz range BJTtransistor or Mosfet
Shikha wrote:
"Can any one suggest me high frequency BJT Transistor or MOSFET available for working with LTspice."
What is your definition of high frequency? For some people, it is 1MHz, for others it might be 10GHz.
To make it a bit easier for you, the following few suggestions have manufacturer-supplied SPICE models: BF998 (N-ch DG MOS) BFR92AW (NPN BJT)
BFT92W (PNP BJT)
Your best bets for SPICE models for RF transistors are the NXP or Infineon websites.?Also, try the group's Files section. I suspect from your question, you haven't actually looked very hard yet.
Regards, Tony
|
Hassan wrote:
? ?"I have found either the .lib file or the symbol !!!?"
That is good.
The first thing to understand is that they are almost completely independent of one another.? A symbol is just an icon, nothing more.? LTspice has some of the symbols already.? In the Select Component (F2) menu, choose the [Misc] area, then you can find DIAC, SCR, and TRIAC symbols.
If you found .lib files, then you found their SPICE models.
Now all you need to do is: (A) include the .lib file in your simulation, and (B) associate the symbol with the model inside the library file.
To include the .lib file, first put the .lib file in the same folder with your schematic that uses it.? Then add this as a SPICE Directive on your schematic:
? ?.lib filename.lib
To associate the symbol with the model:
Right-click on the symbol body and make sure Prefix is set to X.
Open the .lib file in a text editor (such as Wordpad) to see what's inside it.? There should be a subcircuit definition for the part you want to use.? Scroll down until you find it.? It might look something like this:
? ?.SUBCKT 2N6071B MT2 G MT1
Now you know the actual name of the model: 2N6071B.? And you know the order of the pins: MT2, G, MT1.? There could be several .SUBCKTs in the same file, each for a different part.? Find the one you want.
Go back to your schematic.? Edit the name next to the symbol, and change it from "TRIAC" (or "SCR" or "DIAC"), to the name of the subcircuit you want to use ("2N6071B" in this case).
The tricky part is to make sure the order of pins is correct.
For a Triac, LTspice assumes the order of pins is MT2, G, MT1.? If the order differs from that, then you should edit the .lib file and change the pins in the above .SUBCKT line to make them in that order.? This may take a little effort to understand what the pins are, when they don't have those specific names.
Regards, Andy
|
Re: Hello! I want to include/understand the operation of a switch made up of a P_MOS and a N_MOS in parallels and how to assemble them to convert an analogical signal into a numerical signal.Help!
And your LTspice-related question is what?
Regards, Tony
|
Re: high frequency MHz and GHz range BJTtransistor or Mosfet
Hello? Shikha,
NXP has a lot of RF-transistors and they provide SPICE models as far as I remember. Others like Onsemi and Infineon have RF-transistors too.
Best regards, Helmut
|
Re: Current Dependent Voltage Source
" ? rmoreno.phone" asked how to enter a table of measured values for her/his CCVS.
Vlad might have had the table descriptions a little bit confused with respect to your question, because I think the data you have is voltage/current values, not voltage/time values.? You wanted a controlled or dependent source, not an independent source.
Using SPICE's built-in H element (current controlled voltage source or CCVS), LTspice *MIGHT* have the ability to accept a table of current/voltage values.? See the Help pages for E (VCVS) and G (VCCS) elements.? A table is listed as an option. ?"A look-up table is used to specify the transfer function." ?The same 'table' description is not listed for the F (CCCS) and H (CCVS) elements.? I am not sure if that was an omission on those Help pages, or if that option really doesn't exist for those two controlled sources.? The "LTwiki" () is where I usually go when I have questions about the Help pages.? Unfortunately, the LTwiki also doesn't show a table option for the CCVS.? That leads me to believe that you can't use a table with the standard CCVS element.
But LTspice's B-elements can do that and much more.
Here is from the Help page for B-elements:
? table(x,a,b,c,d,...) ??Interpolate a value for x based on a look up table given as a set of pairs of
points.
Start with a Bv symbol, then right-click on "V=F(...)" and edit it.? I think (but could be wrong) it should look like this when you are done:
V=Table( I(V4), 0mA, 0V, 1mA, 1mV, 2mA, 1.9mV, 3mA, 2.5mV ...)
where I(V4) means the current measured through V4 (this is your controlling current), and the pairs that come next, are the (current, voltage) pairs that you measured.
I have rarely used the Table() functions in LTspice, so please excuse my inexperience with them.
Regards, Andy
|
Tony Casey