UP

VIEWING SIMULATION DATA WITH XSCHEM


Usually when a spice simulation is done you want to see the results, this is usually accomplished with a waveform viewer. There are few open source viewers, like GAW...

...Or ngspice internal plotting facilities:

There is also an interesting commercial product from Analog Flavor, called BeSpice (bspwave) that offers a free of charge one year evaluation license for non commercial use:

All these waveform viewers are supported by xschem and more can be added, just by giving the command line to start the viewer to xschem in the Simulation-> Configure simulators and tools dialog:

For gaw and bespice xschem can automatically send nets to the viewer by clicking a net on the schematic and pressing the Alt-G key bind or by menu Hilight->Send selected nets/pins to Viewer

Using XSCHEM's internal graph functions

Xschem can now display waveforms by itself in the drawing area. in the Simulation menu there is an entry to add a graph: Graph -> Add waveform graph. When this menu is pressed a box can be placed in the schematic:

Xschem graphs are embedded into a rectangle object. Resizing graphs is done in the same way as resizing a rectangle object. See the related page. To select a graph (to delete it or move it to a different position) click the left mouse button while in the area shown in this picture:

The next step is loading the simulation data, This is done by menu Waves->Op | Ac | Dc | Tran | Tran | Noise | Sp . This command loads the user selected .raw file produced by a ngspice/Xyce simulation.

Ensure the circuit.raw is saved in binary format (no set filetype=ascii in your testbench)

The raw file is usually located in the simulation/netlisting directory Simulation ->set netlist dir.
After placing a graph box and loading simulation data a wave can be added. If you place the mouse on the inside of the box, close to the bottom/left/right edges and click the graph will be selected. You can also select a graph by dragging a selection rectangle all around it. This tells xschem where new nodes to be plotted will go, in case you have multiple graphs. Then, select a node or a net label, press 'Alt-G', the net will be added to the graph. Here after a list of commands you can perform in a graph to modify the viewport. These commands are active when the mouse is Inside the graph (you will notice the mouse pointer changing from an arrow to a +). if the mouse is outside the graph the usual Xschem functions will be available to operate on schematics:


The graph configuration dialog box which is shown by left button double clicking inside the graph, allows to change many graph attributes, like number of X/Y labels, minor ticks, wave colors, add waves from the list of waves found in the raw file, select the dataset to show in case of multiple sweep simulations and more.

The text area with the colored wave names is just a text widget. You can manually edit it to add / remove waves, or you can place the cursor somewhere in the text, select some waves from the listbox on the left, press the Add button to have these waves added. If you place the insertion cursor in the middle of a node name in the text area, you can click the color radio buttons on the bottom to change the color. The Search entry can be used to restrict the list of nodes displayed in the listbox. The Search entry supports regular expression patterns. For example, ^X will match all nodes that begin with X, xm[0-9]\. will match all nodes containing xm followed by one digit and a dot.

Display bus signals

If you have a design where digital signals are present you might want to group some of these to form a bus and display these bundled signals. After placing a graph box and loading the simulation data as explained above, left-double click the graph to show the configuration dialog, check the bus and digital check boxes, use the Search text entry to restrict the list of signals, then select all the signals you want to show as a bus and click the Add button. Also set the Min value and the Max value of the signals in the bus. This information is needed by Xschem to calculate the logic high and logic low thresholds. Currently the logic '1' is set at 80% of the signal min-max range and the logic '0' level is set at 20% of the signal range. After pressing the Add button a bus is shown in the text area. The first field is a template BUS_NAME that you should change to give a meaningful name to the bus. The bus name is separated from the rest of bits by a , or ; character.

You will then see your bussed signal in the graph:

If you have bussed signals in the schematic , like LDA[12:0] and your graph has the Digital and Bus checkboxes set you can simply add the LDA bus to the graph by clicking the net in the schematic (with the configuration dialog open) and pressing Alt-G:

You can add many signals to see them stacked in a very compact view:

It is possible to switch the graph to analog mode, by unchecking the Digital checkbox in the graph configuration dialog, to better see the waveforms. Switching back to Digital yields the previous view. In analog mode buses are not shown, but are not lost. You will see them again when switching back to Digital mode.

Many graphs can be created in a schematic, and the configuration of all graphs (viewport, list of signals, colors) is saved together with the schematic. If you re-run a simulation just unloading/loading the data from the simulation menu will update the waveforms.

Expression evaluation on waves

It is possible to enter math expressions combining simulation data, for example multiply current and voltage to get the power. The syntax of expressions uses postfix (RPN) notation. When entering an expression use double quotes in the graph edit attribute dialog box, so the expression will be considered as a single new wave to display. Operands are loaded onto a stack like structure and then evaluated. The syntax is:
"alias_name;operand operand operator ..."
Example:
"supply power;i(vcurrvnn) vnn * i(vcurrvpp) vpp * +"
that means: i(vcurrvnn) * vnn + i(vcurrvpp) * vpp.
"i(vcurrvnn) 1e6 *"
that means: i(vcurrvnn) * 1e6.

The optional alias_name is just a string to display as the wave label instead of the whole expression. The following operators are defined:
3 argument operators:

2 argument operators:

1 argument operators:

Display a specific dataset for a node

The following syntax: node%n where node is a saved node or a bus or an expression and n is an integer number will plot only the indicated dataset number. Dataset numbers start from 0. This syntax is accepted for single nodes, bus names and expressions:

"DATA_4; en, cal, saout % 4"
saout%3
"Power dataset 6; I(VVCC) VCC * %6"


Specify a different raw file in a graph

It is now possible (xschem 3.4.5+) to load more raw files for a schematic in xschem.
Each graph may optionally refer to a different raw file. If you double click on a graph while waveforms are loaded you see the graphdialog dialog box:

The dialog box has now a simulation type listbox and a Raw file: text entry box. Specifying an existing .raw file name and a simulation type from the listbox will override the 'base' raw file loaded in xschem. (the 'base' raw file is the only one that was loaded previously and applied to all graphs) If no raw file is specified in a graph it will use the loaded 'base' raw file if any, like it used to work before. It is also possible to have multiple graphs all referring to the same raw file, each graph showing a different simulation. It is for example possible to show a dc, tran, ac simulation all loaded from a common .raw file. Image below shows an example: DC, AC, Transient simulation each one done with 3 runs varying the Bias current. In addition the xschem annotate_op is also used to annotate the operating point into the schematic. Ctrl-Left-button-clicking the Backannotate launcher will instantly update all graphs with data taken from the updated raw file(s).

Specify a different raw file for a single signal in a graph

The general syntax for a signal in a graph is the following:
"alias_name; signal_name % dataset# raw_file sim_type
where:
dataset# is the dataset index to display (only meaningful and needed if multiple datasets are present like in Montecarlo / Mismatch simulations). If empty or -1 then show all datasets.
raw_file is the location and name of the raw file to load. You can use $netlist_dir to quickly reference the simulation directory where usually such raw files are located.
sim_type is the simulation type, like ac, sp, spectrum, dc, op, tran, noise.
Example:
"SAOUT; saout % 2 $netlist_dir/autozero_comp.raw tran


Change sweep variable

The graph dialog box has a Sweep textbox where you can write the X-axis variable. By default xschem uses the first variable in the raw file for the X-axis, and this is the sweep variable the simulation was done, so time for transients, frequency for AC sims, voltage or current sweep for DC sims. Example below shows a cmos latch where a DC simulation has been done sweeping the voltage generator on the a input from 0 to 3V.


If v(a) v(z) is specified in the Sweep textbox (or a z) the z signal will be plotted vs a and the a signal will be plotted vs z.