Keyboard Shortcuts
ctrl + shift + ? :
Показати всі комбінації клавіш
ctrl + g :
Не доступний для безкоштовних груп.
ctrl + shift + f :
Знайти
ctrl + / :
Сповіщення
esc to dismiss
Лайки
Пошук
LM5117
|
alan.spybey wrote:
"I'm a new user, not sure how to get into the Files Section. Is there a model of the LM5117 IC? Thanks " New members should read the instructions they saw when they joined. You get to the Files section by going to the group's webpage and clicking on the word "Files", which ought to be near the top, under the large banner with the schematic and waveforms. (Conversations ... Photos ... Files ...) Or go directly to the Files section's top directory page: https://groups.yahoo.com/neo/groups/LTspice/files To see what models are in the Files section, download the "Table of Contents" file (all_files.htm), open it, and start looking. Use your web browser's search function (usually ctrl-F). I do not see a match for LM5117. (There is a match for LM25117, but it might not be related. Texas Instruments has a SPICE model for the LM5117. Did you try it? Make sure to use only the "unencrypted" model. Encrypted SPICE models are never compatible with other SPICE programs. Regards, Andy |
|
...found these items* (follow-up on Andy;s comments):
https://e2e.ti.com/search?q=LM5117 http://www.ti.com/product/LM5117-Q1 https://www.bing.com/images/search?q=lm5117+schematics&qpvt=LM5117+schematics&FORM=IGRE W. Warren *(download TINA..and then see if a similar chip works there, ...not sure what the matching Linear Tech chip might be..good luck) |
|
Alan, because this model contains a very large number of subcircuits, and you might be new to some of LTspice's features, this is what I recommend doing:
1. Download the unencrypted model from TI. 2. Extract the .LIB file from the .ZIP file. 3. Start LTspice. 4. Drag the .LIB file to the open LTspice window. This opens the model (.LIB) file in LTspice, for editing. 5. Locate this line in the file: .ENDS LM5117_TRANS 6. Move (cut, then paste) that line to the very end of the file. 7. Save the file. 8. Open LTspice's Help. 9. Read this Help page: Schematic Capture > Creating New Symbols > Automatic Symbol Generation. 10. Following step 2 on that Help page, move the mouse down to this line: .SUBCKT LM5117_TRANS HB COMP ... (etc.) and right-click with the mouse on that line, and select Create Symbol. Answer Yes. 11. With the newly generated symbol open, go to Edit > Attributes > Edit Attributes 12. The last line is the ModelFile attribute. Double-click in the Value, and delete the entire path, leaving just the filename, LM5117_TRANS.lib. Press OK. 13. Save the symbol file. Now, just keep the model file (LM5117_TRANS.lib) in the same folder with the schematic that uses it. Alternatively, it could be moved to the correct LTspice subcircuit folder, but you don't need to do that. Regards, Andy |
|
Hi Andy, I definitely am new, and this is really really helpful. Thanks a lot, I’ll give it a go.
Cheers Alan From: LTspice@... [mailto:LTspice@...] Sent: 16 February 2018 04:30 To: LTspice@... Subject: [LTspice] Re: LM5117 Alan, because this model contains a very large number of subcircuits, and you might be new to some of LTspice's features, this is what I recommend doing: 1. Download the unencrypted model from TI. 2. Extract the .LIB file from the .ZIP file. 3. Start LTspice. 4. Drag the .LIB file to the open LTspice window. This opens the model (.LIB) file in LTspice, for editing. 5. Locate this line in the file: .ENDS LM5117_TRANS 6. Move (cut, then paste) that line to the very end of the file. 7. Save the file. 8. Open LTspice's Help. 9. Read this Help page: Schematic Capture > Creating New Symbols > Automatic Symbol Generation. 10. Following step 2 on that Help page, move the mouse down to this line: .SUBCKT LM5117_TRANS HB COMP ... (etc.) and right-click with the mouse on that line, and select Create Symbol. Answer Yes. 11. With the newly generated symbol open, go to Edit > Attributes > Edit Attributes 12. The last line is the ModelFile attribute. Double-click in the Value, and delete the entire path, leaving just the filename, LM5117_TRANS.lib. Press OK. 13. Save the symbol file. Now, just keep the model file (LM5117_TRANS.lib) in the same folder with the schematic that uses it. Alternatively, it could be moved to the correct LTspice subcircuit folder, but you don't need to do that. Regards, Andy |
|
Thanks again Andy, it’s going to take me some time to absorb all your advice ☺
From: LTspice@... [mailto:LTspice@...] Sent: 15 February 2018 23:36 To: LTspice@... Subject: [LTspice] Re: LM5117 alan.spybey wrote: "I'm a new user, not sure how to get into the Files Section. Is there a model of the LM5117 IC? Thanks " New members should read the instructions they saw when they joined. You get to the Files section by going to the group's webpage and clicking on the word "Files", which ought to be near the top, under the large banner with the schematic and waveforms. (Conversations ... Photos ... Files ...) Or go directly to the Files section's top directory page: https://groups.yahoo.com/neo/groups/LTspice/files To see what models are in the Files section, download the "Table of Contents" file (all_files.htm), open it, and start looking. Use your web browser's search function (usually ctrl-F). I do not see a match for LM5117. (There is a match for LM25117, but it might not be related. Texas Instruments has a SPICE model for the LM5117. Did you try it? Make sure to use only the "unencrypted" model. Encrypted SPICE models are never compatible with other SPICE programs. Regards, Andy |
|
Hi I'm uploading a LM5117 spice model and Test circuit. The LM5117 model from TI has some problems, so rather than trying to fix it, I made one from the LM25117 model. The LM25117 model had issues too but was easier to fix. The difference between the two is mainly the supply input voltage range. I'd check the datasheets though. eT |
|
On Mon, Nov 18, 2024 at 01:11 AM, eestudent2025 wrote:
Files > z_yahoo > Files sorted by message number > msg_111329
What sort of problems did you have with it? I trust you used the "Unencrypted" model, right? Any attempt to use one of the encrypted models in LTspice will only fail.
Andy
|
|
Hello, Andy. Thanks for sharing the location of the file.
I was using the unencrypted model by following the steps you provided on this thread but for some reason I kept receiving the error "Too Few Nodes" anytime I tried running my circuit.
Using the "modified" LM5117 model doesn't give me the same error anymore but definitely still not the output I would like.
My goal is to create a Constant Current-Constant Voltage battery charger using the LM5117 buck controller to drive a synchronous buck converter. I have designed my circuit based on the LM5117 datasheet to be able to charge a battery at a maximum of 5A for batteries up to 4.1V. However, this is proving to be quite the challenge for me. Currently, I am only getting about 90mV out.
I will try my best to continue troubleshooting my design. I have uploaded my LTSpice file in case anyone can offer any suggestions or advice. |
|
On Mon, Nov 18, 2024 at 02:30 AM, eestudent2025 wrote:
That should be an easy problem to find and fix. I will look at it later.
In the meantime - you forgot to include these two model files in the ZIP file you uploaded:
PD3S120L.spice.txt
PMEG6010CEH.txt
Without them, I can't try running your simulation. I don't know where those models are needed, but your schematic requires them.
Andy
|
|
On Mon, Nov 18, 2024 at 02:30 AM, eestudent2025 wrote:
I don't know if you want to follow up on that, or just stick with the modified 2017 version from eT (eetech00). If you want to follow up on the "Too few nodes" errors from T.I.'s own model, can you upload your files to the group?
You would have needed to use a different LTspce symbol, of course. The pin-outs of the models are vastly different.
Andy
|
|
On 18/11/2024 14:00, Andy I via
groups.io wrote:
I suspect they are there for a part of the schematic that was deleted before uploading. I just commented out those directives. -- Regards,
Tony |
|
On Mon, Nov 18, 2024 at 02:15 PM, eestudent2025 wrote:
Just to be clear, I think the one you just uploaded is CC_CV_BuckConverter_LM5117_TI_Model.zip .
You forgot to include the symbol file! The missing file is LM5117_TRANS.asy. It's critical that we see that file, because the error is all about a node mismatch between the symbol (.asy file) and the model (.lib file).
Please upload it.
Andy
|
|
Thanks for the updated schematic/files.
I do not have any "Too Few Nodes" error messages when I tried your simulation. I wonder why. More about that later.
However, my simulation did immediately abort because of a shorted voltage source. The error message was:
Fatal Error: Shorted voltage source: u2:v3
That happens because of this element in the LM5117 model from T.I.:
V3 GND 0
In LTspice, node "GND" is synonymous with node "0".
Now that suggests an interesting possibility, that T.I. built the model using a node named "GND" that could be distinct from ground. In LTspice, "GND" is node 0 = ground, so we have a direct short across V3, in LTspice. But it's possible that PSpice does not treat node "GND" the same way.
So, why would there be a separate node "GND" which might not be ground? One possibility is that someone at T.I. wanted to name that node "GND", but leave open the option to either connect it to ground = SPICE node 0, or not. And then V3 makes that connection. Node GND goes to several places inside the model so it isn't trivial to trace it.
I recommend that you edit your LM5117_TRANS.LIB file (the one from T.I.), locate the line with "V3 GND 0", and either delete it or precede it with a comment character ("*").
When I did that, the error was avoided, but LTspice aborted after a few nanoseconds with a "Time step too small" fatal error. If you are unfamiliar with "time step too small" errors, unfortunately they can happen with complex models, and they can be difficult to fix, but it is usually possible to fix them.
Now - the next big question is this: Why do you get errors about "Too Few Nodes", when the model files you uploaded do not have a problem with that?
It suggests that you have files with the same filenames in multiple places, and LTspice may not be using the same files you think it does. In other words, you have a library management problem on your computer.
Andy
|
|
Alternatively, skip trying to use T.I.'s model and go with eT's model instead.
I think he created his LM5117 model from the LM25117 model. I think the LM25117 and LM5117 are not the same; but I did not look into how they differ. But if eT's model works well, I would be inclined to use his.
Also, I forgot to mention that T.I.'s LM5117 model results in a handful of error messages about "curly braces" and "undefined symbols". I am fairly sure that you can ignore those errors. It is possible to "fix" them, but I do not recall seeing a case where it actually made a difference in the waveforms. So it's my belief that LTspice is being somewhat paranoid about those error messages even though it figures it out anyway. (Or I could be wrong.)
Andy
|
|
You are correct! I did have a library management problem with TI's LM5117 model. However, given the remaining issues you mentioned, I have decided to stick with the model that eT made from the LM25117. It appears that these devices are almost identical except for the operating voltage ranges which does not pose an issue in my case. You have been a great help with this, Andy, thank you! |
Tony Casey
Повідомлення
Більше
Додаткові параметри
Більше
to navigate to use esc to dismiss