Hi janstar1122, Welcome to EasyEDA. You have made a couple of simple mistakes that are easy to fix. First though, can I ask that you either: i) make your schematic public as described in: <https://easyeda.com/Doc/Tutorial/introduction.htm#Projectconcept> ii) save it to Anonymous Files and then post the url of the file you have saved it to by copying the url from the browser url bar after you have save d the file: <https://easyeda.com/Doc/Tutorial/introduction.htm#AnonymousFiles> or: iii) share the schematic as described in: <https://easyeda.com/Doc/Tutorial/share.htm#Sharing> That makes diagnosing your problems much easier and more relaible because it saves having to second guess or re-draw your schemaics from scratch. :) **Fixing your problems:** 1) the circuit you have entered into EasyEDA is not wired the same as the one in: <https://dl.dropboxusercontent.com/u/32016513/easyEda/opamp-problem1/AC2.png> You have wired the EasyEDA opamp as a unity gain circuit (R7 should be wired from the inverting input of the opamp to ground and not the output as you have drawn it in EasyEDA). 2) You have set the AC signal amplitude of V2 to 0. You have set the part at the end of the V2 settings as: AC 0 0 where you should have: AC 1 0 Therefore when you run an AC Analysis, you get zero output For more about this please see: <https://easyeda.com/file_view_Spice-Sinusoidal-Source_cw641ZlxT.htm> <https://easyeda.com/file_view_How-to-create-and-run-a-simulation_rVvROaUgs.htm> 3) You have set R8 to 1milliOhm i.e. 1e-3 Ohms when you wanted 1Meg Ohms. In spice (which is the simulator underlying EasyEDA) suffixes are case insensitive so `m` and `M` have the same meaning: 1e-3. To avoid confusion, you have to use `Meg` to represent 1e6. For more, see: <http://ngspice.sourceforge.net/docs/ngspice-manual.pdf#subsection.2.1.3> 4) From your .png, it is not possible to see which opamp you have used. This is one reason it is useful to post a public copy of any schematic you are asking for help on. If you correct the AC amplitude referred to in (2), the suffix for R8 (3) and have used the Parameterised 3 pin Opamp (4) from the EasyEDA Libs, then your sim should run OK. Correcting the connection of R7 to the opamp (1) should then show you your expected Bode plot: <https://easyeda.com/file_view_AC-sweep_GsqnHTfZJ.htm> :)

Hi andyfierman, it was very helpful and now my circuit simulation works correctly. For the record, it is publicly accessible at: https://easyeda.com/project_view_jan-example-circuits_yjhN5dICw.htm I have spent several hours before asking to the forum, so the misplaced resistor, and 0 V AC were my careless mistake for this particular iteration. But the hint to use MEG instead of M - this was the root cause I could not make some of my circuits to work (and others which used only k Ohm did worked) - thous was the source of my frustration . Thanks for your help Jan

Hi, could you help me once more? My next "not working" simulation is the 60-Hz notch filter, posted in the same project: https://easyeda.com/project_view_jan-example-circuits_yjhN5dICw.htm Spice complains about 0 V on resistor R1: Warning: v1: no DC value, transient time 0 value used Warning: singular matrix: check nodes r1_1 and r1_1 The same circuit simulated with the other program worked well: https://dl.dropboxusercontent.com/u/32016513/easyEda/opamp-problem1/AC3.png Would you mind to tell me how to fix this circuit? Thanks Jan

Several problems: i) the TL084N symbol you have chosen from the More Libraries search has no spice model associated with it. It also has 2 hidden supply pins which are unconnected because you have no supply rails. Delete it and replace it with either: the 3 pin parameterised opamp from the EasyEDA Libs and select the parameters to suit your target opamp (see the Properties panel and also read the .subckt netlist to see more details about the 3 pin param opamp model); or: the 5 pin parameterised opamp from the EasyEDA Libs and select the parameters to suit your target opamp and add supply rails (see the Properties panel and also read the .subckt netlist to see more details about the 5 pin param opamp model). or: the 5 pin opamp from the EasyEDA Libs and in the Properties panel, edit the name from opamp5pEE to TL081EE. Make the name visible if you wish. Add supply rails. (Also, read the .subckt netlist to see more details about the 5 pin opamp model). 2) Somehow the schematic is corrupted because when you delete U1.3 and replace it with the 3 pin opamp, the wire from opamp pin8 to 9 just vanishes. I don't know why and I have raised a bug report with Dillon. You may be best deleting the whole of the Vout net, adding the new opamp and then redrawing the Vout net. (See:< https://easyeda.com/file_view_Probing-voltages-01_Il5nTDx3z.htm> for more about voltage probes and how they generate - and in some cases, overwrite - net names). 3) You have no DC path to ground at the opamp non-inverting input. You cannot run a real opamp like this because there must be a DC path to ground for the input bias current to flow through (sorry, I can't locate a good article about this on the web right now). Since EasyEDA opamp models are designed to mimic real world behaviour of opamps, the model throws an error without such a resistor (though this has pointed out that I may need to slightly modify the opamp models so that instead of throwing an error, the circuit just does what a real circuit would do, which is cause the output to saturate at one rail or the other). Adding a resistor from the junction of C1 and C2 (or at the opamp non-inverting input) will then make the sim run but bear in mind that this will change the frequency response. It's also good practice to make the total DC resistance seen by the inverting and the non-inverting inputs, the same to cancel out dc offsets caused by the input bias current offset.

This might help: <http://www.rficdesign.com/opamp-parameter>

This is an excellent article about avoiding common mistakes and problems in circuit designs using opamps: [Designing Amplifier Circuits: How to Avoid Common Problems] [Designing Amplifier Circuits: How to Avoid Common Problems]:http://www.analog.com/static/imported-files/application_notes/AN-937.pdf