First of all, I manually entered a netlist with a simple circuit with a single transistor. For this, I used the syntax that SPICE expects to receive and I obtained the operating point of the circuit.
Secondly, I entered the same circuit using the schematic and checked the generated netlist. As you can see in the attached figure, there are some differences that I have highlighted that I think are different from the standard SPICE syntax. I don’t know if any of you would be so kind as to explain the differences to me (especially the one referring to the QMOD transistor).
However, the results obtained from the operating point for each of the ways of introducing the circuit are exactly the same.
As always… Thank you for your time!
You can get same results in these two simulation only because BF and IS in the .model QMOD set to default value. In your schematic, you didn’t correctly config your transistor, you are just calling a default transistor to use and not QMOD defined in your .model.
In string attribute
Name : Qnnn
1st attribute : model name
NPN is an instance parameter for bipolar transistor (this parameter is not accepted by spice program likes LTspice, if to run a Qspice netlist with transistor in other spice program, you can use “;” to comment NPN section, or delete it from netlist). According to HELP in Qspice, instance parameter NPN is to invoke an error if used with a PNP .model. This NPN is automatically added, if Symbol Type is QN.
If you force Symbol Type from QN to Q (type Q in Symbol Type in Symbol Properties), automatically generated netlist will remove NPN from it.
For .lib NPN.txt, it is the standard library link in using Symbol Q. If you delete it from Library file, this line will be removed from automatically generated netlist. As this is Q spice library, if you need your netlist to run in other spice, you may consider to copy NPN.txt library to the schematic folder or with that model copy into schematic and comment this library path.
In Symbol Type, type a Q and press Enter
In Library File, delete NPN.txt
Thank you KSKelvin!
Interpreting the Qspice HELP, in my case, is not always an easy task (but there we are!), therefore, the help you and others offer with clarifying examples is a great help. Thank you.
I updated my device reference guide for Qspice with BJT model parameters. This guideline is just to give a rough idea of instance or model parameters in affecting the device performance. As you are studying BJT parameters, hope you can find it useful. Please refer to this link to download this pdf.
Device Reference Guide by KSKelvin.pdf at KSKelvin-Github/Qspice