I was trying import OPA547 model (pspice model from TI)
Simulation shows weird results, any help?
Attaching schematic files and model files
OPA547.txt (4.6 KB)
Expected out was 400mVpp with 200mVpp Sine input. All kind of weird errors.
Model and test bench circuit works fine in Pspice and TINA TI. Didn’t try LTSpice
When you are adding new model. Check include entire file.
Already tried with no luck
Not an easy fix like adding entire file. I feel, entire Pspice Syntax is not supported by QSPICE
your failure is your fault. In order to turn on the op-amp, a voltage higher than 2.4 V must be applied to pin 7. You should read the datasheet carefully!
The operational amplifier is good. Thank you for drawing my attention to it. Spice is a good model!
When I review OPA547 Pspice model, I found an issue related to transistor in Qspice. Not sure if this is the cause, but just reported to Mike for review.
I read it completely. As per datasheet, pin 7 can be left open or apply voltage above V- + 2.4V.
Even if you apply voltage above, Qspice shows error.
I am sure Mike will fix it.
which version of Qspice you are running?
The version I am running with QSPICE64.exe Build on Oct 7 2023 15:17:56
with latest revision history as
10/07/2023 Implemented HSPICE-style BJT model parameters IBE and IBC.
If goto HELP > Simulator > Device Reference > Q. Bipolar Transistor
Run the example Qexample.qsch in Q. Bipolar Transistor
You will see collector current vs base current of NPN transistor is not correct currently.
My feeling is that this problem is the reason why OPA547 is not working currently.
this is how this example performed currently. In DC sweep, collector voltage goes to 0V but still have collector current.
What modifications did you do to make it work?
I am running latest version of QSPICE
Take a look at how you turned R1 on and how I turned it on.
But the accidentally revealed problem with the bipolar transistor model is also very important!
I won’t be updating the program for now until the bug is fixed.
Understood. But I am not drawing any current from output stage. So this shouldn’t be a problem.
Lets wait for the bug fix.
Mike fixed an error in BJT model in today update.
10/07/2023 Fixed an error in the implemented of the HSPICE-style BJT model parameters IBE and IBC.
For OPA547 Pspice model from TI, you can auto generate symbol with or without select the checkbox of Include Entire File. Include Entire File is required if sub-circuit contains other sub-circuit, but for OPA547, it didn’t call other sub-circuit. So, hopefully, the problem you encounter was just coincidentally met a bug as on previous version introduce IBE and IBC parameters but broke the BJT model. Update Qspice and it works fine now.