Hello.
I have this transistor and many others in my model collection.
Here is the link:
http://bordodynov.ltwiki.org/
Download the lib.zip file
Read how to add my models.
I have this transistor and many others in my model collection.
Here is the link:
http://bordodynov.ltwiki.org/
Download the lib.zip file
Read how to add my models.
A quick question: how can I apply the .FOUR function to the difference of two voltages in the schematic? I would like to get the Fourier components of the AC voltage between the ends of a center tapped transformer.
Deleted... wrong answer from me 🙂 I see you wanted the difference, not both results showing together.
I solved it by adding an ideal transformer with the secondary ground referenced.
Attachments
Sometimes it pays to be stubborn. Yes, you can FFT a difference:
1. to just do the error log, just direct ".four {f} V(a,b)"
2.1 to plot a difference fft, start with view FFT in the trace dialog but select two nodes by control clicking the second node.
2.2 This brings up a dialog that allows you to select and edit the selected nodes, including an expression with Alt-double-click, which can be V(a)-V(b) or V(a,b)
2.3 click OK
1. to just do the error log, just direct ".four {f} V(a,b)"
2.1 to plot a difference fft, start with view FFT in the trace dialog but select two nodes by control clicking the second node.
2.2 This brings up a dialog that allows you to select and edit the selected nodes, including an expression with Alt-double-click, which can be V(a)-V(b) or V(a,b)
2.3 click OK
Attachments
I am wondering if some people also have these very bizarre issues every so often?
Starting with a totally fine and working, but rather complex simulation.
Changing a few things causing the simulation the totally stall.
Okay, fine, going back to the original by undo, or deleting parts, simulation still doesn't work.
Quitting en reloading the original schematic, everything is totally fine again?
Totally beats me....
Starting with a totally fine and working, but rather complex simulation.
Changing a few things causing the simulation the totally stall.
Okay, fine, going back to the original by undo, or deleting parts, simulation still doesn't work.
Quitting en reloading the original schematic, everything is totally fine again?
Totally beats me....
A software bug, most likely a memory leak. You can try reporting the bug but the chances of being taken seriously are small if you are an individual hobbyist. The bug reporting process (initiated through the "Help / About" menu) gets a reply asking for your name, company, etc. before AD will provide any support. At least that has been my experience.
Good luck!
Good luck!
Even as a professional (working with/under several bigger companies) the response to any bug reports is 0%
Yes, I have seen similar. It's not necessarily a bug. Simulation uses recursive loops to converge onto the results, and it is easy to create a near infinite loop, which uses up your memory and then goes to disk cashing which takes forever so it essentially hangs. The transformer post ~3230 is an example where it seems the problem is partially floating nodes that causes simulation to take ~forever. Treating SPICE as a black box is problematic. Everything needs a ground reference. You could argue that the software should detect a problem and throw an error, and sometimes it does, but maybe bulletproof is impossible.
SPICE 2G6 used to issue the despised message "NO DC PATH TO GROUND FROM NODE abcdef" then refuse to proceed. Users hated this so much that the non-open-source derivatives of 2G6, which were sold for money and not given away for free like Berkeley SPICE, eliminated the message and performed lots of behind-the-curtain shenanigans to make these (degenerate) circuits appear to simulate.
Hi All
I did see all the models for irf6645 series from infinion do not work wel. I get just +- 40 volts out of the bridge
and I have a supply of 60 volts x 2. Other models do work but need low Nc..
Also the irs20124 model do not work if i set VCC to the negative voltage as normal needs to be done, only at gnd it works.
thanks for help.
I did see all the models for irf6645 series from infinion do not work wel. I get just +- 40 volts out of the bridge
and I have a supply of 60 volts x 2. Other models do work but need low Nc..
Also the irs20124 model do not work if i set VCC to the negative voltage as normal needs to be done, only at gnd it works.
thanks for help.
Attachments
Last edited:
maybe you can share the ltspice file as well as the models, kind of hard to see what's going on this way?
Course I did forget, here the are. The mosfet I did make the whole set, irf6645 is there. IRFB4020pbf do fine
als others but need low nC. IRF does shoot through 540 amps also, I think it is because of wrong model.
Thanks for looking at it.
als others but need low nC. IRF does shoot through 540 amps also, I think it is because of wrong model.
Thanks for looking at it.
Attachments
I'm having trouble with the bipolar transistor files in LTspice. It seems there have been changes in the last few years in the system structure. I wanted to add a transistor to standard.bjt. However every trick I have tried (that used to work) doesn't anymore. The file now is under LTC in programs instead of users. It need admin to edit but the edits don't show up suggesting I'm editing the wrong file or that the list of available parts is coded somewhere else. Its also seems a lot have been removed looking at older versions of the files.
I would like to use this file as my standard.bjt if I can get it to work: http://ltwiki.org/index.php?title=Standard.bjt Any advice?
I would like to use this file as my standard.bjt if I can get it to work: http://ltwiki.org/index.php?title=Standard.bjt Any advice?
I recommend you find the free download, free-to-use software called "Everything" , published by voidtools dot com. Install it on your Windows machine and use Everything to find each and every file called standard.bjt . It will surprise you how many there are. Edit each and every one of them to include all of your non-Analog-Devices model statements. Victory.
Initially still no success just finding the instances. BUT a sync release to update all the files and then determine that the active file is in the C:\Program Files\LTC\LTspiceXVII\lib directory based on file dates. Then start LTspice as administrator, open the file, edit and save (you need administrator privilege's to do this). Its all more complicated than it should be today. The punch card history of spice still hangs over it.
In any case I can now reverse engineer this Burleigh PZ-70 "high voltage opamp" (up to 1500 volts out) to extend its response from 1KHz to 100 KHz hopefully.
In any case I can now reverse engineer this Burleigh PZ-70 "high voltage opamp" (up to 1500 volts out) to extend its response from 1KHz to 100 KHz hopefully.
C:\Program Files\LTC\LTspiceXVII\lib is not the place for you. You need administrator privileges to access it. Now it's more convenient and you don't need admin rights! Now you have a new folder with models available to you
C:\Users\uswrname\Documents\LTspiceXVII\lib
Go to my web page
http://bordodynov.ltwiki.org/
C:\Users\uswrname\Documents\LTspiceXVII\lib
Go to my web page
http://bordodynov.ltwiki.org/
It can be handy to include your own models in the "select another transistor" dialog by editing C:\Users\%userprofile%\Documents\LTspiceXVII\lib\cmp\standard.bjt but then you need to add ~"Vceo=30 Icrating=800m mfg=NXP" to each model and it is vulnerable to updates.
In most cases, the part has already been selected so you just need to list the model
1. placed on the schematic as a .model directive
or
2. in an included file which can be a text file anywhere on your computer
or
3. ".incl" or ".lib" a URL pointing to a library such as Bob Cordel's or Minek's web sites. This automatically download the library file into your downloads folder if you care to move it later.
An advantage of 3rd party library files is that LTC will not mess with them during updates, and you can put it where there are no security problems. It may be useful to add a path in the control panel:
In most cases, the part has already been selected so you just need to list the model
1. placed on the schematic as a .model directive
or
2. in an included file which can be a text file anywhere on your computer
or
3. ".incl" or ".lib" a URL pointing to a library such as Bob Cordel's or Minek's web sites. This automatically download the library file into your downloads folder if you care to move it later.
An advantage of 3rd party library files is that LTC will not mess with them during updates, and you can put it where there are no security problems. It may be useful to add a path in the control panel:
Attachments
The surest way to avoid updating is to add a suffix. I had this problem with JFET transistors. I found that some factory models don't model flicker noise well (or rather don't model at all). I tweaked the models, but after a while I found that I had the original models. So I made new models with the _n suffix added. For example LSK389A_n.