1. LTspice
  2. Теми

problems with unknown subcircuit

 

Hello,

I know this question has been asked a hundred of times, but I still quite can't figure out, what is wrong with my circuit.

When I run the simluation I get the error message: Unknown subcircuit called in..  

I am still fairly new to LTSpice, so I really hope someone may help. I have upload the schematic to:

Temp/LTSpiceAnalogesBackend_upload

 
 

Please don't upload multiple files into a new folder in Files > Temp. It is nauseatingly tedious to download each one individually.

Please put everything in a zip file (not any other kind of compressed archive) before uploading. Then, we have just one download to do.

--
Regards,
Tony




On 20/11/2024 11:25, kodphil via groups.io wrote:

I know this question has been asked a hundred of times, but I still quite can't figure out, what is wrong with my circuit.

When I run the simluation I get the error message: Unknown subcircuit called in..  

I am still fairly new to LTSpice, so I really hope someone may help. I have upload the schematic to:

Temp/LTSpiceAnalogesBackend_upload
 

You also haven't included a "pwm" symbol.

We can't help you until you have uploaded everything necessary.

--
Regards,
Tony

On 20/11/2024 13:52, Tony Casey wrote:

Please don't upload multiple files into a new folder in Files > Temp. It is nauseatingly tedious to download each one individually.

Please put everything in a zip file (not any other kind of compressed archive) before uploading. Then, we have just one download to do.

--
Regards,
Tony




On 20/11/2024 11:25, kodphil via groups.io wrote:

I know this question has been asked a hundred of times, but I still quite can't figure out, what is wrong with my circuit.

When I run the simluation I get the error message: Unknown subcircuit called in..  

I am still fairly new to LTSpice, so I really hope someone may help. I have upload the schematic to:

Temp/LTSpiceAnalogesBackend_upload
 
Змінено

kodphil,
 
Your 74HC04 symbols look like a mess.  They have:
  • Value = 1
  • Value2 = 1
  • SpiceLine = 1
  • SpiceLine2 = 1
which makes absolutely no sense, and it is probably the cause of your problem.  Get rid of all that trash which doesn't belong.
 
Then you stuck some parameter definitions ".param vcc1=1 speed1=1 tripdt1=1" below them, but they are not parameters of those symbols so they might not be handed to those symbols, and it isn't right.
 
But more to the point - why did you create your own symbol for the 74HC04, when you should have used the one inside 74HC.zip which you should have downloaded from the 74HC library folder?  Not only does that symbol look like a 74HC04 inverter, but it has the correct nodes and the correct parameters to make that device work.
 
Perhaps you made other mistakes too, but the above ones were the obvious ones.
 
Also -- please don't upload any *.OLB files (they are for PSpice, not LTspice), and please no PDF files either unless they can't be found anywhere on the Internet.
 
I cleaned up your uploaded files.  You need to deal with the rest.
 
Andy
 
 

To elaborate a bit more about the cause of your error:
 
By using your unnecessary 74HC04 symbols with Value, Value2, SpiceLine, and SpiceLine2 all set to "1", it netlists like this:
    XU1 pwm pwm_n VCC 0 74HC04 1 1 1 1
LTspice looks at that and understands that it is a subcircuit call, to a subcircuit named "1", because "1" is the last name on the end of 8 nodes.  And there is no subcircuit defined with the name "1".  So that is what caused the error message.
 
Your schematic seems to be loading a lot of unnecessary SPICE models.  I may be wrong.   But why do BSS84.txt and BSS138.txt need to be included?  Are they used anywhere?
 
Andy
 

1 - 5 з 5