You may need to use BV, if you can try to find more information via https://easyeda.com/Doc/Simulation-eBook/index.htm ![enter image description here][1] [1]: /editor/20151121/565001638ce16.png

Please see: https://easyeda.com/Doc/Simulation-eBook/Configuring-Voltage-and-Current-Sources.htm#ConfiguringVoltageandCurrentSources https://easyeda.com/Doc/Simulation-eBook/Setting-up-Analyses.htm#SettingupAnalyses and: https://easyeda.com/Doc/Simulation-eBook/Expressions.htm#Expressions :)

Please also see: https://easyeda.com/Doc/Simulation-eBook/Parameters.htm#Parameters https://easyeda.com/Doc/Simulation-eBook/Functions.htm#Functions https://easyeda.com/Doc/Simulation-eBook/B-sources.htm#Bsourcesspicesimulation

Thanx so far, folks. But: My schematic returns a WaveForm when pressing Ctrl+R. Including this in a text box: tran 0.200ms 0.200s 0.000s uic .param + Faktor=27 + PWatt={Faktor}*{I(vxPROTOR)} + SWatt={Faktor}*{I(vxSROTOR)} + PRegler=0 + SRegler=0 prevents a WaveForm from showing up. None of these parameters being used in any component yet. Just setting them according to the instructions in the manual causes trouble.

The editor of this site altered the regular "*" to a dot.

Can't see your schematic, so you may need to try to remove some parts one by one until to dig the problems.

I did remove parts to turn the schematic down to a very simple state. Setting .ic values correctly does not help. I make the schematic public now, so maybe someone can help. The circuit is about comparing the standard generator system of the old BMW airheads to a modified one. I need the diagrams.

@dillon Schemativ is published now.

There is an ammeter named PROTOR. The value of the current it measures is to be multiplied by 27. There is also a volProbe and a resistor to calculate the current. The result of this multiplication is to be used as the parameter Amplitude(A) of a current source. Can anyone tell me how to get this done, please ? Show me the way to do it with a correctly written syntax, please ? By now I suspect the manual to be badly written... Using a function as a parameter of a current/voltage source ??? No way !!! It's getting sort of boring to follow the instructions in the manual in detail without any positive result.

Tommy, Sorry you're having trouble getting started with your simulation. Let me try to explain some of the reasons that your sim is not working and offer some suggestions as to how to fix it. There are a number of problems in your schematic - which I will try to explain below - but some are because you have not been able to find the correct information on our site. The reason for this is partly because there are some issues in the Table of Contents of the **Simulation eBook** which I am working to resolve but you can download a copy of the whole html document from here: https://drive.google.com/file/d/0BxSnqhiCbZEjRXNfaHl4UXkyejFhRF9GbzBXMWNlLVlGT1Y0/view?usp=sharing Once downloaded, if you just click on the html file, it should open in your browser (or just drag and drop the file into a browser window or tab). * Your B2 Behavioural Source uses an ifx() function which will not work because you have not copied and pasted the function that this calls up from the example in the eBook. This is because this section of the eBook is broken on the EasyEDA website. * The expression you have used in B2: V=ifx(v(vPRotor)<14.4,0,v(DPlusP)-v(vPRotor)) will fail because you have referred to the voltage on a net, V(DPlusP), which does not exist in your schematic. I suspect you mean **V(DPlus_P)**. * Your **param** statement for: .param + OutputP=Stator(I(PROTOR)) is broken because it does not netlist correctly. You have entered: .param on a line of text and then made it into a spice directive and then you have entered: + OutputP=Stator(I(PROTOR)) on a separate line of text and then made it into a spice directive. above the .param line you have created the spice directive: .func Stator(x) {x*27} These three lines have ended up being incorrectly parsed as: .param .func Stator(x) {x*27} + OutputP=Stator(I(PROTOR)) and not as: .func Stator(x) {x*27} .param + OutputP=Stator(I(PROTOR)) which is what you intended. When you enter a spice directive, it can be spread over several lines *but all the lines must be in the same text block when you turn them into a spice directive*. * The **.func** function definition statement: .func Stator(x) {x*27} whilst it is syntactically correct, serves no purpose because you have not then placed the function, Stator(x), in a B source. * However, the **.param** parameter assignment: OutputP=Stator(I(PROTOR)) is incorrect because: i) you cannot assign a dynamic value (in this case the current through an ammeter) to a variable (in this case OutputP). To achieve that you must use a B source in a similar way to that which you have already implemented for B1. ii) you cannot refer directly to an ammeter by using the name of the ammeter. You must prefix the name with VX as you have done in the expression you have used in B1. A simpler way to refer to the current in series with something is to insert a 0V voltage source and then you can refer to the voltage source directly by name. Alternatively, you can use a Current Controlled Voltage Source or a Current Controlled Current Source. Please see: >https://easyeda.com/Doc/Simulation-eBook/Introduction-to-using-a-simulator.htm#Probingsignals in the Simulation eBook (or the same section in the standalone html version) * Something I would suggest is that, until you are familiar with working with spice and the syntax of the many different statements and function, you work through the examples in the eBook and then apply them, building up to your final simulation a step at a time.