Helmut Sennewald 05/08/12 #54296
--- In LTspice@..., "VincenzoV" <varoli@...> wrote:
I have uploaded the file log_amp.zip. When I try to simulated this circuit I get the error message of the title. This happen only with a PC with Windows7. On another PC also with Windows7 and on a PC with WindowsXP the file does no give this error message but only a warning that in the subcircuit of the opamp ADA4898 there is a node with only one connesion.
WARNING: Less than two connections to node U9:9. This node is used by E:U9:CMR.
Even with this warning the simulation results seem good. All the PC use the 30 april version of LTspice. I do not understand the reason of this different behavior. Thanks in advance and best regards.
Vincenzo Varoli
Hello Vincenzo,
Your "ada4899.cir" has a missing comment "*" in the first line or you have to use .lib instead of .inc.
Your file
source ADA4899
.SUBCKT ADA4899 INV NINV OUT VCC VEE
...
Good file
* source ADA4899
.SUBCKT ADA4899 INV NINV OUT VCC VEE
...
I can think of only one reason why it works on the other PCs. The PCs it works may have a "good file" in the installation folder. Don't put any of your files into the installation folder.
Best regards,
Helmut