Unknown subcircuit problem in LTSpice when using Encrypted Vendor Device Library

Thread Starter

Sitara

Joined May 2, 2014
57
I have downloaded and unzipped an encrypted mosfet library from Fairchild (ONSemi). The file is called ONSemi_SUPERFET2_600V_LTspice.zip. This library is specifically meant to be used with LTSpice. The zip file contains device schematic symbol files (xxxxx.asy, where xxxxx is the device name), one file for each device in the lib, as well as a text file named ONSemi_SUPERFET2_600V_ltspice.txt. This txt file is, presumably, the encrypted *.lib file containing the spice parameters of the devices.

Below is a cut and paste of the start of this text file:

upload_2017-3-7_17-46-28.gif

The Hex code at the bottom of the screen dump above, continues for the remainder of the file.

I copied the unzipped directory containing the *.asy & *.txt files into the LTSpice\lib\cmp directory and then attempted running a simple simulation using one of these mosfets. LTSpice produced an unknown subcircuit error. Here is a screen dump of the circuit schematic and the error message:
upload_2017-3-7_17-53-25.gif

What do I need to do in order to successfully run the simulation ? Many thanks in advance!
 

Thread Starter

Sitara

Joined May 2, 2014
57
hi Sitara,
Please post your LTS asc file so that we can try it out.
Also the model files.
E
Hi Eric,
I have tried a number of times to upload the schematic file. I get this error message:

upload_2017-3-7_18-56-9.gif

What must I do to succeed in uploading?
 

Alec_t

Joined Sep 17, 2013
10,604
I copied the unzipped directory containing the *.asy & *.txt files into the LTSpice\lib\cmp directory
Try putting the .txt file in the \lib\sub directory.
If using LTspiceXVII under Win10, that directory should be in the Documents path.
 

Thread Starter

Sitara

Joined May 2, 2014
57
Try putting the .txt file in the \lib\sub directory.
If using LTspiceXVII under Win10, that directory should be in the Documents path.
I'm using LTSpiceXVII under Windows 7 64bit OS. I just tried out your suggestion. Unfortunately, LTS cannot see the devices when the library is put into \lib\sub directory.
 

eetech00

Joined Jun 8, 2013
1,740
I have downloaded and unzipped an encrypted mosfet library from Fairchild (ONSemi). The file is called ONSemi_SUPERFET2_600V_LTspice.zip. This library is specifically meant to be used with LTSpice. The zip file contains device schematic symbol files (xxxxx.asy, where xxxxx is the device name), one file for each device in the lib, as well as a text file named ONSemi_SUPERFET2_600V_ltspice.txt. This txt file is, presumably, the encrypted *.lib file containing the spice parameters of the devices.

Below is a cut and paste of the start of this text file:

View attachment 121999

The Hex code at the bottom of the screen dump above, continues for the remainder of the file.

I copied the unzipped directory containing the *.asy & *.txt files into the LTSpice\lib\cmp directory and then attempted running a simple simulation using one of these mosfets. LTSpice produced an unknown subcircuit error. Here is a screen dump of the circuit schematic and the error message:
View attachment 122000

What do I need to do in order to successfully run the simulation ? Many thanks in advance!
Hi

To make sure the files work, unzip the .zip file and copy/move all the unzipped files into the same folder as the your schematic.
Use the include statement on your schematic to include the .txt file.
Place the symbol on the schematic then change the symbol "Prefix" property to "X" without the quotes.
Should be good to go.
 

Thread Starter

Sitara

Joined May 2, 2014
57
Hi

To make sure the files work, unzip the .zip file and copy/move all the unzipped files into the same folder as the your schematic.
Use the include statement on your schematic to include the .txt file.
Place the symbol on the schematic then change the symbol "Prefix" property to "X" without the quotes.
Should be good to go.
Thank you eetech00 !! That did the trick! And here is the proof of the pudding:

upload_2017-3-8_1-16-32.gif
 

Thread Starter

Sitara

Joined May 2, 2014
57
Thank you eetech00 !! That did the trick! And here is the proof of the pudding:

View attachment 122015
Is there a way of 'generalising' or increasing the scope of a device library beyond its containing folder, say by including a path in the include statement, of the form:
.include c:\directory01\directory\02\directory03\Libraryname.lib
so that we needn't have to make local copies of device libraries (in the directory containing the circuit schematic), particularly for circuits which use a number of non-(LTSpice standard library) parts whose libraries are scattered in different directories ?
Edit: Yes, adding path works. I've just checked. That way you can keep the libraries in a fixed location and reference them using the path portion of the .include statement. The device schematic symbols can remain in subdirectories of the the LTSpice\lib\cmp directory and can be selected using the Add part icon or F2.
Edit2: I meant to say subdirectories of the LTSpice\lib\SYM directory, in my previous edit.
 
Last edited:

eetech00

Joined Jun 8, 2013
1,740
Is there a way of 'generalising' or increasing the scope of a device library beyond its containing folder, say by including a path in the include statement, of the form:
.include c:\directory01\directory\02\directory03\Libraryname.lib
so that we needn't have to make local copies of device libraries (in the directory containing the circuit schematic), particularly for circuits which use a number of non-(LTSpice standard library) parts whose libraries are scattered in different directories ?
Edit: Yes adding path works. I've just checked.
Hi

Yes.
You can configure paths to be searched when adding a symbol.
Look at Control panel->"Sym & Lib search paths" tab.

Add .asy file paths in the Sym pane.
Add subcircuit paths in the Lib pane.

After that, place your files in the corresponding locations..

Here is an example of how I've structured folders and specified paths:
Sym pane (.asy files stored in each folder):
d:\ltc\lib\sym\74HC
d:\ltc\lib\sym\74HCT
d:\ltc\lib\sym\CD4000

Lib pane(subckt files stored in each folder):
d:ltc\lib\sub\74HC
d:\ltc\lib\sub\74HCT
d:\ltc\lib\sub\CD4000

After specifying the paths, you can specifiy just the .lib file without the path in the .include statement on your schematic.
 
Last edited:
Top