ltspice cannot find its own opamp

[istemihan]

Hi everyone,
I am dealing with an electronic circuit. It has a small non-inverting and inverting circuit inside. They had opamps but ltspice cannot recognize its own opamp. It gives me error : "Unknown subcircuit called in: xic7 n001 n009 n008 n010 n004 p001 ltc6268-10 " . I uninstalled the LTspice from my computer and installed again but there is no change. Indeed, If I draw another basic circuit with this opamp It works. If you have an idea please help me.

 

[MikeMl]

Post your .asc file

 

[istemihan]

.asc file
these are written in its log file

Missing ".ends" statement in file "deneme1.net"
Questionable use of curly braces in "vcc4 n010 0 {v}"
Error: undefined symbol in: "[v]"
Questionable use of curly braces in "vee2 0 n004 {v}"
Error: undefined symbol in: "[v]"
Questionable use of curly braces in "vcc3 n011 0 {v}"
Error: undefined symbol in: "[v]"
Questionable use of curly braces in "vee1 0 n003 {v}"
Error: undefined symbol in: "[v]"
Questionable use of curly braces in "vcc1 p002 0 {v}"
Error: undefined symbol in: "[v]"
Questionable use of curly braces in "vcc2 p001 0 {v}"
Error: undefined symbol in: "[v]"
Questionable use of curly braces in "vcc5 n002 0 {v}"
Error: undefined symbol in: "[v]"
Circuit: * Z:\home\zehra\LTspice\week10\deneme1.asc

WARNING: Trouble expanding subcircuit "ltc6268-10"
Fatal Error: Unknown subcircuit called in:
xic7 n001 n009 n008 n010 n004 p001 ltc6268-10

 

[alec_t]

Where did you get the LTC6268-10 model from? It's not in the opamps folder that LTC installs.
Is the model intended for a different spice? It includes uplim and dnlim functions which I've not come across before.

 

[istemihan]

I got it from LTC/lib/sub direction inside the LTC6.lib folder. This opamp is one of the opamps which LTspice includes. But I had same problem a few days ago for an ordinary LTC opamp -OPA07- . I thought that If I reinstall LTspice It might improve but it is not.

 

[eTech]

Where did you get the LTC6268-10 model from? It's not in the opamps folder that LTC installs.
Is the model intended for a different spice? It includes uplim and dnlim functions which I've not come across before.

Hi
LTC6268-10 is my Default LTspice library...
Also...uplim and dnlim are undocumented but valid LTspice functions.

 

[eTech]

.asc file
these are written in its log file

Missing ".ends" statement in file "deneme1.net"
Questionable use of curly braces in "vcc4 n010 0 {v}"
Error: undefined symbol in: "[v]"
Questionable use of curly braces in "vee2 0 n004 {v}"
Error: undefined symbol in: "[v]"
Questionable use of curly braces in "vcc3 n011 0 {v}"
Error: undefined symbol in: "[v]"
Questionable use of curly braces in "vee1 0 n003 {v}"
Error: undefined symbol in: "[v]"
Questionable use of curly braces in "vcc1 p002 0 {v}"
Error: undefined symbol in: "[v]"
Questionable use of curly braces in "vcc2 p001 0 {v}"
Error: undefined symbol in: "[v]"
Questionable use of curly braces in "vcc5 n002 0 {v}"
Error: undefined symbol in: "[v]"
Circuit: * Z:\home\zehra\LTspice\week10\deneme1.asc

WARNING: Trouble expanding subcircuit "ltc6268-10"
Fatal Error: Unknown subcircuit called in:
xic7 n001 n009 n008 n010 n004 p001 ltc6268-10

Try this one...

 

[istemihan]

Thank you so much !

 

[eTech]

Thank you so much !

Here's what I did to fix it:

1. Removed and re-added LTC6268-10, U1, component using the component selector.
Probably didn't have to do this but left it that way.
2. Removed the LTC6268-10 .subckt statement from the schematic. It wasn't needed.
3. The diode was defined twice with two .subckt statements on the schematic.
I commented out the first line like this:
*.subckt D 1 2
4. Assigned "PMLL4448" to the value field of each diode.

 

[alec_t]

LTC6268-10 is my Default LTspice library...
Also...uplim and dnlim are undocumented but valid LTspice functions.

Oops. Found it (must have had my eyes closed before!). Thanks for the info re those functions.

 

[istemihan]

Hi everyone,

I have same problem again with another circuit. "unknown subcircuit" why is it happening? I couln't figure out! Now I am trying an basic opamp differentiator amplifier circiut. I try to understand behaviour of an opamp but i could not make it. It tells unkonwn subcircuit for opamp. Could you please tell me how will I deal with this unknown subcircuit problem? .lib file is in ltc library and also in the same folder with .asc file.

 

[MikeMl]

What folder is opa857.lib in?

 

[istemihan]

I put the spice file of opa857 in ltc' library (sub) and I also put spice file and .asc file are in same folder.

 

[MikeMl]

Post the file: opa857.lib

 

[istemihan]

It did not send the file with .lib so I wrote it as .sub

 

[MikeMl]

That is not a valid Spice subcircuit. That is a model for TI's stupid WebBench...

 

[istemihan]

thank you for your help. my major is not electronic but i try to learn so i am sorry i could not recognize it. now i learn what is a webbench. thank you again.