# Simulation aborted because there are errors during netlisting

Tags:
1. Oct 21, 2012

### jean28

I have built the following circuit:

http://i1226.photobucket.com/albums/ee410/jean28x/pspicemodel.jpg

However, when I try to simulate it, I get an error that says "Simulation aborted because there are errors during netlisting. Please refer to the sessions log."

What am I doing wrong? I'm new with PSPice so i'm not sure what's wrong.

Thanks.

2. Oct 21, 2012

### Simon Bridge

Did you refer to the sessions log and read the errors?

3. Oct 21, 2012

### Kholdstare

Where did you go wrong?

Mine ran just fine. You have selected 'ac analysis/noise' in simulation profile, right?

#### Attached Files:

File size:
29.7 KB
Views:
996
• ###### 2.jpg
File size:
49.8 KB
Views:
846
4. Oct 22, 2012

### Jony130

Why you circuit don't work? The answer is simply you forgot about power supply. Unpowered opamps DO NOT WORK!

5. Oct 22, 2012

### jean28

I hadn't selected the Noise in simulation profile. I select AC Sweep/Noise analysis and then which options to I select? The frequency es 10000 Hz so I know that but what do I put in the Noise analysis part?

6. Oct 22, 2012

### jean28

I ran it while changing options in the noise area and got this mistake:

7. Oct 22, 2012

### Jony130

You must be kidding me.
Your circuit will work if you add symmetric power supply to op amp. Positive terminal to pin 4. Negative to pin 11 and GND to ground.

8. Oct 22, 2012

### Simon Bridge

It usually helps someone follow your advice if you show how you came to the conclusions you did. What made you realize that the power supply was not hooked up correctly?

9. Oct 22, 2012

### Simon Bridge

Code (Text):
*Analysis directives:
[b].AC DEC 100 10000 1000[/b]
------------------$ERROR -- Invalid value [b].NOISE 10 50[/b] -------$
ERROR -- Must be independent source (I or V)
What do the three numbers in the .AC directive mean?

10. Oct 22, 2012

### Jony130

Just one look at the diagram

And what you see ?? No power supply.

Are you sure?? Output voltage is only 42μV. Typical example of GIGO in the case of simulators, garbage in=sophisticated garbage out.

#### Attached Files:

• ###### bez tytułu.JPG
File size:
20.7 KB
Views:
6,627
Last edited: Oct 23, 2012
11. Oct 22, 2012

### Simon Bridge

Could this have something to do with the second error message?

12. Oct 22, 2012

### davenn

what the 6.25V AC ? thats the input signal me thinks

D

13. Oct 22, 2012

### Simon Bridge

This is what I'm talking about! Now what role has OP got it playing in the circuit diagram?

Probably best to continue this part of the discussion in private since it is about how to answer questions effectively and not actually about OPs problem.

14. Oct 22, 2012

### Kholdstare

You dont necessarily have to put noise analysis in your simulation if that is not something you want to do.

15. Oct 22, 2012

### Kholdstare

Code (Text):
.AC DEC 100 10000 1000
------------------$ERROR -- Invalid value .NOISE 10 50 -------$
ERROR -- Must be independent source (I or V)
The ".AC" command syntax is
Code (Text):
.AC <sweep type> <points value> <start frequency value> <end frequency value>
In your case start freq is greater than end freq. You have to set it correctly in simulation window.

The ".NOISE" command syntax is
Code (Text):
.NOISE V(<node> [,<node>]) <name> [interval value]
You did not give V(output node) and name(noise source) etc.

I'm telling you again, you probably do not need noise analysis. So turn it off. AC analysis will run just fine without noise analysis.

16. Oct 22, 2012

### Kholdstare

Jony, I know very well that the circuit will not work hooked up like that. But that does not mean the circuit will not simulate and give out the garbage value. The issue I tried to solve was with the simulation procedure. Once that is done Jean can see whether his circuit produces desired result or not, and come to us again.

17. Oct 22, 2012

### vk6kro

I tried a LTSpice simulation of this circuit.

Because of the positive feedback, the output depends on the initial voltage on the input, but it always goes to one supply rail or the other.

Assuming this is a mistake, I reversed the inputs to the opamp and it then behaves like a low pass filter with a 6dB cutoff of about 300 Hz.

As a matter of interest, if the 10 nF capacitor is replaced with a smaller value, the circuit becomes a bandpass filter. For example, a 220 pF capacitor in this position produces a peak output at about 1480 Hz.

Last edited: Oct 23, 2012
18. Oct 23, 2012

### Jony130

This is not true. This circuit (correct diagram) is a multiple feedback low-pass filter.
And if you change capacitor to 220pF the only think that has change except cut-off frequency is a quality factor. Q has change from 0.7 to Q = 4.767 for 220pF but it is still a low pass filter.

#### Attached Files:

File size:
4.7 KB
Views:
374
• ###### 11.PNG
File size:
2.5 KB
Views:
409
19. Oct 23, 2012

### vk6kro

Without the dB scale, it looks like this:

http://dl.dropbox.com/u/4222062/LPF%20BPF.PNG [Broken]

This is the 100 pF output.

So, although the circuit LOOKS like a low pass filter, it behaves like a band pass filter because it has the wrong components in it to be a proper LPF.

I mentioned this because this filter can apparently cover quite a large section of the audio spectrum with a small variable capacitor. So, it is interesting because it has some applications.

Last edited by a moderator: May 6, 2017