Click the image to get the sch-rnd sheet; also requires this project.lht in the same directory
In this simulation we are going to calculate the DC operating point of a simple voltage divider. This is also an introduction to setting up a sheet for circuit simulation and setting up the high level simulation infrastructure.
The single-sheet schematic contains the voltage divider with all networks named. There are no extra symbols for the simulation, the circuit is in its original form, as designed for the PCB workflow.
In SPICE simulation there are different analysis options available: these are different simulation actions or operations or modes. Basically each analysis is a different algorithm to run on the circuit. The simplest analysis is called the "DC operating point analysis".
In the op point analysis, the simulator will apply all sources, assume all inductors are shorted and assume all capacitors are open and then calculate the voltage for all nodes. (Node is the spice terminology for an equipotential electrical network.) This simulation is not time or frequency dependent, and represents a single DC operating point once the circuit has already stabilized.
In our example, this means 5V would be applied at CN1 then out1 and out2 are calculated. Since our voltage sources are ideal and capable of supplying any amount of current, the voltage on the in network will be 5V; but the voltages on out1 and out2 will depend on the resistor values of R1, R2 and R3.
Draw the schematics as usual; make sure there is a gnd network, spice won't work without that. Ideally, use the stock gnd symbol for that. Make sure all resistors have a unique name and a value. Spice understands the normal SI suffixes such as k for kilo, but as it is generally not case sensitive, m and M are both milli, so you will need to write meg to get mega.
Your symbols also need to have the proper spice pin numbers. First switch your view from the default pcb to sim_ngspice: there's a button for this on the top right part of the main window, on the left of the help/support button. This pops up a view selector; click sim_ngspice twice and the selector will close and the view will change. The new view will show pin numbers as seen by the spice target. For plain resistors, pin ordering does not matter, but it is important for polarized parts like diodes, transistors, and sources. The stock library has spice pin numbers set up and should work without modification. Later chapters of this tutorial will explain how to deal with spice pin numbers in symbols.
Using the sim_ngspice view CN1 and CN2 are crossed out with red. This means these symbols are not exported: spice can not simulate connectors. This happens because the attribute spice/omit is set to yes on these symbols. The stock library has spice/omit set on mechanical symbols.
The message log also has an error message saying that modifications could not be applied to the sim setup because there is no active simulation setup. This is normal when sim_ngspice is manually selected, which is the rare case. Normally a simulation setup is activated from the simulation setup dialog and that configures everything properly.
High level simulation needs to store a lot of simualtion-specific configuration: different simulation setups, different output (e.g. plot) options. Since many real life designs use multiple sheets, these can not be stored on the sheet level but has to be stored on the project level. Thus the high level sim feature always operates on the project level and always stores configuration in the project file, project.lht. This is true even on the single sheet case.
The dialog box for the high levle sim feature is accessible through the File menu, Project... submenu, Circuit simulation submenu. This opens the Simulation selector dialog, presenting a set of different simulation setups (or sim setups for short). Different sim setups will simulate
A typical use case is to have a sim setup for evaluating the board in the simplest DC case and a few other sim setups exploring how the circuit works with different AC stimulus. Another typical use case is to take a complex circuit apart and simulate different stages separately - this can be done without adding any extra symbols or other clutter in the drawing, only by high level sim configuration.
In this example, and in most of the examples, there would be only one simulation, to keep things simple. Click on that one item on the list to select it and click the Open... button. (This sim setup was once created by clicking the New... button, which asked for a name for the new sim setup, created it blank, and then opened the same sim setup dialog described below.). Sim setup names are arbitrary user assigned strings, only to help the user remember which sim setup is for what (sch-rnd is not basing any decision on the name).
This opens the simulation setup dialog for the selected sim setup.
The sim setup dialog has 3 tabs and a control block on the bottom. Each tab is configuring an important aspect of the given simulation setup and is going to be described in detail below.
The first tab defines the circuit that is going to be simulated:
This is equvalent to the process of physical testing of a circuit: once the basic circuit is built as documented by the schematics, optionally a part of it is isolated for testing (this is called test benching in sch-rnd) and external stimulus, probes and sometimes artifical connections or loading resistors and alike are added for the measurement (this is the modifications part).
Select the only item in the modifications tableand click the Edit button. This opens the modification editor that shows:
Or in short: this is the 5V power supply connected to CN1.
The advantage of having this as a modification instead of drawing it as a voltage source symbol on the sheet is the less visual clutter on the drawing, especially when not dealing with simulation. It is also more natural to say "connect 5V to CN1 for this test" than to draw symbols of non-existing parts.
This advantage pays off even more when there are multiple different simulation setups each having different sources installed at random parts of the circuit. Without modifications, all sources of all simulation setups would need to be added to the drawing (or on separate "test bench sheets").
Note: CN1-2 uses component name - port name; port name means the name the port is listed by in the abstract model, which is typically the original terminal name, and not the "pin number", or the calculated display/name attribute. In case oc CN1-2, port name and "pin number" or display/name happens to match, but for example using a polarized symbol, e.g. a diode it is typically A and C (not 1 and 2); or using a transistor symbol, the port names are B, E, C (and not 1, 2 and 3). Tip: switch to the raw view to reveal the original port names or use the abstract model dialog to find them.
The second tab, output config, defines the spice analysis to execute and how the results are presented. A single simulation setup can define multiple output, in which case each simulation is ran on the given setup, in the order they are specified, and are presented in the same order. This is useful to get multiple printouts or plots of the same or different analyses.
Select the first entry, which runs the 'op' analysis and presents the result simply printing values. Click on the edit button. This opens the sim output config dialog. The top half of the dialog box configures the analysis; the op analysis does not have parameters so it's sparse in this example. The bottom half configures the presentation, which is set to 'print' in this case, which will simply print the textual value of any property listed. The list can be edited using New/Edit/Remove buttons. Each item of the list is a network name or a component-port pair (or a function based on one of these). In this example we are measuring voltages at two pins of connector CN2.
The third tab presents simulation results. Before the simulation is first ran, this tab is empty. Click on the 'run' button in the bottom control block of the dialog box; the 'run' button will activate the sim setup (selects the sim_ngspice view and sets all sim related configuration) and run the simulation (ngspice) in the background and fill in the third tab once the simulation finishes.
In this simple example the output will contain:
CN2-3 = 2.38095238e+00 CN2-2 = 1.19047619e+00the voltages measured on pin 3 and 2 of the connector CN2, as requested in the output config.
