|
Hello, I Have imported the TH3491 PSPICE LIB file and made it into a symbol by using the subckt create symbol command ,the LIB file is in the folder below.I wanted to check the TH3491 opamp as a buffer.
The part of the circuit where its being used is shown in the photo link below.
The lspice file and symbols are attached in the folder link below
I have this error shown below.
When i remove the TH3491 component there is no error with the spice model of BZT52C3V6
Missing ".ends" statement in file "C:\Users\yefimv\Documents\pulse shaper\BZT52C3V6.spice"
LTspice 24.0.12 for Windows
Circuit: * M:\ltsims\74ABT04_pulse_shapr_double_split_3.asc
Start Time: Sat Jul 20 11:54:04 2024
Warning: Multiple definitions of model "2scr375p" Type: BJT
Warning: Multiple definitions of model "bc857b" Type: BJT
Warning: Multiple definitions of model "bc847c" Type: BJT
Warning: Multiple definitions of model "bc847b" Type: BJT
U1:2:m6: all pins shorted together -- ignoring.
LTspice circuit photo:
https://groups.io/g/LTspice/photo/294510/3807606?p=Created%2C%2C%2C20%2C2%2C0%2C0
LTSPICE file and symbols folder:
https://groups.io/g/LTspice/files/Temp/john23/ths3491
https://www.ti.com/product/THS3491?bm-verify=AAQAAAAJ_____7xIuOxy2V0jDpcKcJnSM1KK_N5zGjJ6_i-yWWWhljsFiqb2jTYo0udDmIeSAUDARa9Zonv3z44E4X5jabOOpOkkXjT3H8jr_v2N7sqPS2J37njKPqk4oW1ZMMoY81hr4GoAghR0zm9HcYRc4LhEH7AmVRKkFNNxjNb9gGQTf6_SMMR16Mu1ogy8UOcjRoy1VKkna7u_o_9b7ZID8AiJO39uKb8ikdN6pbx7Tx7xrPV7iB63r-l0-c4PEEGWR-K0cgw9LCO-E8T1T9D0WNsm1FXTcm6psrxxYhUjDPPBls0zVLB5-J5vNw2ARKZjgGc
|
See below.
On 2024-07-20 09:56, john23 wrote:
Hello, I Have imported the TH3491 PSPICE LIB file and made
it into a symbol by using the subckt create symbol command ,the
LIB file is in the folder below.I wanted to check the TH3491
opamp as a buffer.
The part of the circuit where its being used is shown in the
photo link below.
The lspice file and symbols are attached in the folder link
below
I have this error shown below.
When i remove the TH3491 component there is no error with the
spice model of BZT52C3V6
Missing ".ends" statement in file
"C:\Users\yefimv\Documents\pulse shaper\BZT52C3V6.spice"
Open the file in LTspice and add the 'Ends' statement, then save
it.
LTspice 24.0.12 for Windows
Circuit: * M:\ltsims\74ABT04_pulse_shapr_double_split_3.asc
Start Time: Sat Jul 20 11:54:04 2024
Warning: Multiple definitions of model "2scr375p" Type: BJT
Warning: Multiple definitions of model "bc857b" Type: BJT
Warning: Multiple definitions of model "bc847c" Type: BJT
Warning: Multiple definitions of model "bc847b" Type: BJT
Ignore these warnings.
U1:2:m6: all pins shorted together -- ignoring.
Check your .ASC and remove the short.
--
OOO - Own Opinions Only
Best Wishes
John Woodgate
Keep trying
|
Your upload is missing ABT04 and LMH6654 symbols. It is also missing
the abtpnom.lib model library. There is probably more missing but
LTspice only tells you one at a time.
If you want people to help you, you must ensure every uploaded
schematic has all the files that didn't come with LTspice are
included, preferably in a single zip file.
Don't expect people to dive back into your previous uploads, of
which there are many, to attempt to find the missing files. You
should do this work so that others don't have to.
"Warning: Multiple definitions of model "2scr375p" Type: BJT" and
similar lines in your Error Log are not errors, and won't affect
your analysis.
--
Regards,
Tony
On 20/07/2024 10:56, john23 wrote:
|
Quite apart from the other issues raised regarding you latest
schematic, the THS3491 is a current feedback amplifier and cannot be
successfully used as voltage follower. You must understand how
current amplifiers work to successfully use them.
Why are you trying to use this part?
--
Regards,
Tony
On 20/07/2024 10:56, john23 wrote:
Hello, I Have
imported the TH3491 PSPICE LIB file and made it into a symbol by
using the subckt create symbol command ,the LIB file is in the
folder below.I wanted to check the TH3491 opamp as a buffer.
|
On 20/07/2024 12:40, Tony Casey wrote:
You
must understand how current amplifiers work to successfully use
them.
..current feedback amplifiers..
--
Regards,
Tony
|
john23 wrote: "When i remove the TH3491 component there is no error with the spice model of BZT52C3V6"
I do not believe it. The error message about the BZT2C3V6 model is due to your BZT52C3V6 model (which you failed to upload). Removing the THS3491 would not affect that error, unless you also deleted that diode from your schematic. Did you?
re: "U1:2:m6: all pins shorted together -- ignoring."
I can't find U1 on the schematic you uploaded. That is what causes that message. I think it is the ABT04 device, whose symbol and model you failed to upload, so I can't check it to see why it has a short-circuit. But anyway, it's probably "safe" to ignore that warning message. What LTspice is telling you is that transistor M6 inside that device is shorted out (all its pins connected together), so LTspice took M6 out of the simulation. That's harmless - although one might want to know why transistor M6 was included in U1's model but shorted out and whether that was intentional.
The four warning messages about "Multiple definitions" of BJT models can be ignored. Those happen because Analog Devices has failed - for years! - to fix their transistor model file. Analog Devices was sloppy and the file contains multiple definitions of those four BJT models. You will get those four warning messages any time your simulation has at least one BJT (PNP or NPN) transistor, and those warnings won't happen if your simulation has no BJTs. The warnings probably also indicate that you have not updated your LTspice libraries since you installed it. You should do that.
Why do you continue to use a schematic that you know is flawed? We have discussed parts of that schematic already, and at least two of us pointed out a fundamental design mistake that you made on that schematic - and yet you ignored our advice and failed to fix it. Why? Are you just wasting our time? Please don't do that. When we tell you that your schematic has a design flaw, you should fix the design flaw and not continue to bother us with the same mistakes, weeks later.
What is the point of the red markings on the Photo you uploaded? Do they mean something?
Andy
|
john 23's reply says, "Missing ".ends" statement in file "C:\Users\yefimv\Documents\pulse shaper\BZT52C3V6.spice""
In the BZT52C3V6 model that you uploaded here two weeks ago (BZT52C3V6.spice), I can see the problem. The last line of that file is this:
.MODEL DR D ( IS=11.4f RS=74.5 N=3.00).ENDS
which is supposed to be two lines, but somehow the linefeed between the two lines got deleted and it turned into one line. That is why LTspice could not find the ".ends" statement. It was "hiding in plain sight."
The end of that file should look like this:
.MODEL DR D ( IS=11.4f RS=74.5 N=3.00)
.ENDS
Edit your copy of that file and fix it, and that warning message will go away.
That message has nothing to do with the TH3491 (or THS3491 which is the actual part number), except maybe because of their relative order in your SPICE Netlist file. Apparently you have been living with that mistake for weeks and didn't notice it before. Depending on the exact order of lines in the SPICE Netlist file, it might have gone unreported.
Andy
|
I changed the Subject line to correct the part number. The part is a THS3491, not TH3491. There is no TH3491.
Andy
|
Hello, I have uploaded ABT04.asy LMH6654.asy abtpnom.lib attached in the folder.(i will zip all the files together) Thanks.
|
On 2024-07-20 at 21:02 john23 via groups.io wrote:
Hello, I have uploaded ABT04.asy LMH6654.asy abtpnom.lib attached
in the folder.(i will zip all the files together)
Why did you not use the temp folder as described in the Group rules?
Important: ... upload
files to the "Temp" folder - https://groups.io/g/LTspice/files/Temp
.
The way to keep all files together is easy:
Put all necessary files in the same folder and use file links (e.g.
.lib or .inc) without path prefix.
Bernhard
|
Yes, as has been stated many times, don't add 3rd party files to the LTspice folders - that's the root of your problem. If you do that you will never know which files your uploads are missing, because your system always finds them.
For maximum portability, keep all required files in the same folder as the schematic. Then just zip up the folder, and it will contain everything necessary.
Duplication shouldn't be an issue so long as you don't change any of the files.
Lastly, you should learn how to use the symbols already provided by LTspice with 3rd party models, like the 3.6V Zener you keep using. LTspice has a perfectly good Zener symbol that everyone will recognise for what it is.
Try not to auto-generate a symbol for every model you use. Auto-generated symbols always cause problems with schematics you share.
-- Regards, Tony
On 20 Jul 2024 21:02, john23 <yafimvar@...> wrote: Hello, I have uploaded ABT04.asy LMH6654.asy abtpnom.lib attached in the folder.(i will zip all the files together) Thanks.
|
john23 uploaded files to an odd location in the group's files. They have now been moved to a subdirectory of the "Temp" folder, here:
Files > Temp > john23 > ths3491 > missing
re: "Is there a way i could see if anything will be missing?"
It requires thinking about what your have.
- Every LTspice simulation starts with a schematic (.asc) file.
- On that schematic, there are several symbols (.asy files). Symbols are not part of the schematic; they must also be provided. All LTspice users have the symbol files that came with LTspice. Any symbols that didn't come with LTspice need to be uploaded by you.
- Most symbols also have a SPICE model. All LTspice users have the SPICE models for everything that came with LTspice. For every component that did not come with LTspice, you must locate and upload its SPICE model. Some symbols have the name of the SPICE model embedded within the symbol itself, but some do not.
- Every ".inc" or ".lib" command loads another SPICE model. Those must be uploaded by you.
Therefore, you need to stop and think, what things do I have in my simulation that were not part of LTspice itself? What things did I download, or create? You need to spend a few minutes thinking about what those things are, locating them on your computer's drive, and then including them with the schematic when you upload it.
For everyone concerned, the simplest thing to do is to ZIP all those files together into one .zip file - make sure that it is .zip and not anything else - and then upload just that one .zip file. Upload it directly to the " Temp" folder and nowhere else.
If you have access to a second computer, you can do this:
- Install LTspice on that second computer.
- Do not install any other SPICE symbols or models on it.
- Take the .zip file that you created above, copy it to the second computer, unzip it there, and try to run the simulation of that schematic.
- If it doesn't work, then you left something out. Go back and find the missing files and add them to the .zip file.
Andy
|
Correction: "All LTspice users have the symbol files that came with LTspice."
|
john23,
You have not yet uploaded these files:
- "tssop.s". Your schematic has a command ".LIB tssop.s" to load that file, but the file is still missing.
- "abtpnom.lib". Your schematic has a command ".LIB abtpnom.lib" to load that file, but the file is still missing.
- "LMH6654.LIB". It is the SPICE model for the LMH6654 that is on your schematic. The symbol you created for the LMH6654 shows that the file is located on your computer's drive, here: "M:\ltsims\New folder\LMH6654.LIB". It needs to be uploaded. (Either that, or the simulation could be simplified by removing the LMH6654. Don't try doing too many things at once.)
There might be others missing too, but these three were obvious.
It is already challenging for us because you auto-generated some symbols, unnecessarily, and every time you auto-generate a symbol, the symbol embeds the exact location of its SPICE model within the symbol. That makes it not portable to anyone else's computer. We all need to edit your auto-generated symbol files to remove those exact locations.
There was no need to auto-generate a symbol for a zener diode (BZT52C3V6). LTspice already has a zener diode symbol.
There was no need to auto-generate a symbol for the LMH6654. LTspice already has a generic 5-pin op-amp symbol; it's called "opamp2", and MOST OF THE TIME it has the same pin-order of the SPICE model so it can be used with MOST op-amps.
The THS3491 is different because it has extra pins, so a new symbol was needed for that part.
Andy
|
Hello, regarding what you said.
Is there some manual(video will be great)so i could use to show the proper way how to generate a symbol so it will be portable?
https://www.ti.com/lit/zip/sbombp9
Thanks.
On Sat, Jul 20, 2024 at 11:02 PM, Andy I wrote:
It is already challenging for us because you auto-generated some symbols,
|
john23 asked, "Is there some manual(video will be great)so i could use to show the proper way how to generate a symbol so it will be portable?"
I do not know if there is a video for this, and sorry but I am not going to make one. But here are the extra steps:
- Create the symbol using the usual steps on the "Automatic Symbol Generation" help page. I assume you know how to do that because you made some already.
- With the symbol still open in LTspice, press Ctrl-A (or go to Edit > Attributes > Edit Attributes).
- If the symbol is not still open in LTspice, then locate the symbol again (it is probably in LTspice's [AutoGenerated] folder), open it in LTspice, and now press Ctrl-A.
- The "Symbol Attribute Editor" now appears on the screen.
- Look for the "ModelFile" attribute. It is the last one in the list.
- Double-click on the value in the ModelFile line.
- Edit it to remove everything before the filename.ext. The only thing left should be the filename.ext of the SPICE model file that you started with.
- Click OK.
- Save it. (Click the Save icon, or go to File > Save.)
That is all you really need to do, to make that symbol portable. By deleting the "path" to the file's location which exists only on your computer, now it can work on other computers too.
Now you need to make sure that the SPICE model file can be found. A good place to put the SPICE model file, is in the same directory where you are running the simulations that need it. LTspice can always find it if it's in the same folder with the schematic, if its filename is unique.
But that might be a challenge if you plan to be running many simulations located in many different folders. You can put a copy of the same SPICE model file in each of those folders. Or you could put the SPICE model file into a specific folder where LTspice always looks.
- You could put that SPICE model file into LTspice's own lib\sub folder, but I do not recommend it. Yes it works, but I think it is best to leave LTspice's own lib\sub folder with LTspice's own model files only. Your added model files ought to go somewhere else.
- LTspice lets you add "Sym. & Lib. Search Paths", which are lists of directories that YOU own and control, and LTspice will check there when it runs simulations. The SPICE model is a Library file, not a Symbol file, so add it to the Library Search Path.
Andy
|
John Woodgate
Tony Casey