Looking at this resource it seems that it depends where you put the GND: [https://www.youtube.com/watch?v=EkHch86UXpY&t=1064s](https://www.youtube.com/watch?v=EkHch86UXpY&t=1064s) EasyEda force you to set at least a GND, the problem probably is where I set the GND but I am not sure.

@sasadangelo, It will help you to read the **Simulation Tutorial** (3) in (2) in: [https://easyeda.com/forum/topic/How-to-ask-for-help-and-get-an-answer-71b17a40d15442349eaecbfae083e46a](https://easyeda.com/forum/topic/How-to-ask-for-help-and-get-an-answer-71b17a40d15442349eaecbfae083e46a) i.e. 3) If you wish to **Simulate** your design then you **must** also read the: [Simulation Tutorial](https://docs.google.com/document/u/1/d/1OWZVVFRAe_2NW3WratpkA_SGuHa5AcRow5ZRfvcoVTU/pub) * This is a temporary link while the document and the examples are being updated for LTspice compatibility Where you have set your ground is correct for measuring the output side of the transformer. Assuming that the voltage into it is a pure sinusoid with an RMS value of V(ina,inb), where V(ina,inb) is the voltage difference across the input terminals of the bridge rectifier, you are correct in that the peak voltage out of a bridge rectifier with a fixed forward drop of 2*0.7V is ``` V=uramp(sqrt(2)*ABS(V(ina,inb))-1.4V) ``` where ABS(x) is the absolute value of x and uramp(x) is a function that gives 0 for x LT 0 and x for x GTE 0. If you netname the inputs to the bridge as **ina** and **inb** then you can try replacing your bridge rectifier with a B source using the expression above. There are however, a number of things that affect the measurements you are making in your sim. 1. The value of 0.7V forward drop for a silicon diode is an approximation. It depends on the current through the diode. At zero current there is zero drop and it then increases in proportion to the log of the forward current plus the I*R drop due to the bulk resistance of the diode so at higher currents the drop becomes dominated by the IR drop. Check the datasheet for the GBJ1504 bridge rectifier. Then look closely at what happens around the zero voltage troughs of the output voltage with a 10k - and compare that with - a 10 Ohm load resistor. 2. The DMM has an input resistance of 100G Ohms so on its own it still draws a small - but compared to the 10k load - negligible current. 3. The representation of the waveforms is somewhat limited by the way spice works. The waveforms are not perfectly smooth so there will be a small error associated with the linear approximations:  4\. There are other small errors in the **.measure** statements that are used to supply the measurements to the DMM display. You can see these statements in the window that opens when you click on the **Show your simulation report** button: 

Hi, First of all, thank you for your reply. Obviously I read the tutorial but I don't think it could help me with my doubts. My doubt is first of all theoretical (and probably we agree that this is the right place to post the problem), but then there is a practical doubt that is related to EasyEda. Your answer to my first doubt seems to confirm with my surprise that formula 1) is valid (see my original question). Then this means that the 1.4 V drop must be calculated on Vrms in input to the bridge and not Vp or Vpp. Is my understanding correct? If so, the transformer output is 12 Vrms so the Vp at the bridge output should be: (12V-1.4V)*sqrt(2)=14.94. Looking at EasyEda it gives me 16.3Vp. Now I understand that there could be some tolerance on diode drop voltage and that there are other small errors here and there, but the error is more than 1V. Are you telling me that this is normal in EasyEda? It's not a critique, it's just to understand what to expect from the tool. Thank you for support.

Sorry, above I meant that this is NOT the right place to post the theoretical problem, but it is for the practical.

Sorry again, forgot my reply above. Looking better at your formula: ``` V=uramp(sqrt(2)*ABS(V(ina,inb))-1.4V) ``` you remove 1.4V to Vp that is sqrt(2)*abs(Vrms). Looking better at this formula I have: Vrms=12.115 -> Vp=sqrt(2)*12.115=17.13->remove from this the drop voltage->17.13-1.4V=15.73 -> EasyEda show a value around 16.3Vp but this is ok because we have to consider that drop voltage could change with load (I have 10K load) and there is some tolerance on how EasyEda tracks the curve. Multimeter measure RMS value so I have: Vrms=Vp/sqrt(2)=15.73/1.41=11.12 that is very close to the value of 11.49 I see on the display. Do you think my understanding of how things works is OK now? Thank you in advance for your support, you really help me to understand how things work on EasyEda.

It may be simpler just to think of the 1.4V just as being subtracted from the absolute value of the instantaneous input voltage to the bridge for all input voltages greater than 1.4V than. To talk about RMS and peak voltages can get very confusing because the RMS and the peak of the voltage out of the bridge may be very different from that of the input depending on load current and the amplitude of the input compared to the bridge drop. :)

Ok thank you

Looking to the datasheet I see Vfm 1.05, does this mean that the max Volt drop is 1.05V? [https://www.diodes.com/assets/Datasheets/ds21219.pdf](https://www.diodes.com/assets/Datasheets/ds21219.pdf)

Another thing I noticed is that the wave in output to the transformer is 0.5V (almost) less than GND this is the reason the wave becomes negative (-0.5V) at the minimum. This is a thing I have never found in theory books.

@sasadangelo, 1.05V @ 7.5A per diode:  so the total drop with 7.5A flowing through both conducting diodes in either polarity is 2.1V. "...the wave in output to the transformer is 0.5V (almost) less than GND this is the reason the wave becomes negative (-0.5V) at the minimum." If you think about it you will see that this must be so in order that the -ve output side diodes in the bridge can conduct:  "This is a thing I have never found in theory books." Yes, I have found this too. It is obvious once you have seen and thought about it but it can be very confusing until you do and most books and presentations about AC circuits with bridge rectifiers do not point this out. A lot of the confusion is because you don't always think about where the voltages are measured with respect to which is why I make a point about this issue in the Spice Tutorial. If you move the ground net to one of the transformer AC outputs and then look at the WaveForm plots it all looks absolutely crazy but all you have done is moved the reference point for all your measurements to a different and probably unfamiliar point. Sometimes in spice simulations you need to move the ground to an unfamilar place to make sense of the waveforms and then maybe move it back to look at some others and what is even more confusing is that sometimes spice fails to converge with a ground in one place yet is fine with it in another. There are reasons for this and if you want to know more I recommend reading: [http://ltwiki.org/index.php?title=Convergence_problems?](http://ltwiki.org/index.php?title=Convergence_problems%3F) and the sections on Convergence is John Warner's excellent documentation for SIMetrix: [https://help\.simetrix\.co\.uk/8\.3/simetrix/simulator\_reference/topics/convergence\_accuracyandperformance\_transientanalysis\.htm\#What\_Causes\_Non\_convergence\_](https://help.simetrix.co.uk/8.3/simetrix/simulator_reference/topics/convergence_accuracyandperformance_transientanalysis.htm#What_Causes_Non_convergence_) Sometimes all that is needed is to reverse the order of a capacitor in series with a resistor and suddenly the convergence problem goes away! Crazy but you get a feel for it after a while.

You're great and very kind. I don't want abuse of your patience and for now, it is OK for me. Thank you very much. Just FYI I decided to do some simulations on the diode and Graetz bridge alone just to better refresh my electronic study in high school almost 25 years ago. I loved Electronic for a long time but then I abandoned for Software Programming because at that time to build an electronic circuit you needed to find materials, design the circuit to find out only at the end that reality is not always like theory. A few years ago I restarted my old passion because I could leverage on software simulation easy to use, I tried DoCircuits.com for some time but it was full of limitation and I abandoned it (the company disappeared). Tried Spice but too complex. Now EasyEda seems the right tool for me and thanks to this tool I am starting to understand Spice too (I already tried some circuits). My goal is to put my old theoretical knowledge into practice to design circuits using first simulation tool and when I have a good project tested I want to try to order a PCB and build it. I would like to start with a simple Power Supply -15/+15V 2 or 3 A with a digital voltmeter (I know there are a lot of circuits around the web but I want to test my knowledge and only at the end compare the result with a real circuit). Then move to amplifiers (I remember I designed and built a couple of them 25 years ago) and radiofrequency. Thanks again for your support, I really appreciated it.

There are lots of sims that I have put up here for peopple just like you to play with... :) In the following sims, just ignore the messages like this (it's a bug, it's been reported) and just click OK:  [https://easyeda\.com/example/Tesseract\_Guitar\_Practice\_Amp\_simulation\_files\-H0ca8IFDB](https://easyeda.com/example/Tesseract_Guitar_Practice_Amp_simulation_files-H0ca8IFDB) [https://easyeda.com/example/Uberclamp_simulation-RzsmgyQ8q](https://easyeda.com/example/Uberclamp_simulation-RzsmgyQ8q) Here are some simpler examples: [https://easyeda\.com/andyfierman/Projects\_for\_beginners\-tqkewO60i](https://easyeda.com/andyfierman/Projects_for_beginners-tqkewO60i) but they do not yet all run because in trying to update them to run on LTspice, I have discovered a raft of bugs... one of which explains your confusion in one of your earlier posts over using what you thought - quite correctly - to be a B Source!

Thank you. They seem very advanced for my knowledge but I'll consider them for the future.

One simple question, it is outside from the scope of this thread, but why every time I start a new project I notice that some symbols disappear from EE Lib and I need to cut & paste them from other schemas? How EasyEda decides which element show in EELib, this is another thing very confuse. I know I can search them in Libraries, but it's really confusing. I can understand that for space, not every component can be shown in EE Lib but sometimes very basic one disappear Zener (see my other thread), multimeter, power source, and so on.

@sasadangelo, The contents of the EELib changes depending on whether you are  creating a "passive" non-simulation schematic (Std mode) or an "active" simulation schematic (Sim mode) but those are the only changes there should be. Can you post some screenshots to show that? For more about the differences between an "passive" non-simulation schematic or an "active" simulation schematic, please see (2.1) and (2.2) in (2) in: [https://easyeda.com/forum/topic/How-to-ask-for-help-and-get-an-answer-71b17a40d15442349eaecbfae083e46a](https://easyeda.com/forum/topic/How-to-ask-for-help-and-get-an-answer-71b17a40d15442349eaecbfae083e46a)

This might explain some of it...  :)