PREV UP NEXT

# 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.

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 `set graph_use_ctrl_key 1` is set in the `xschemrc` file all bind keys shown below will need the `Control` key pressed to operate on the graphs. This setting can be used to make it more explicit when the user wants to operate on graphs. Without the `Control` key pressed the usual functions on schematic are performed instead of graph functions.
Example: the key `a` will create a symbol if used in a schematic while it shows a cursor if done when the mouse pointer is inside a graph. With the `set graph_use_ctrl_key 1` option you will need to press `Control-a` with the mouse pointer inside a graph to show a cursor.

if the mouse is outside the graph the usual Xschem functions will be available to operate on schematics:

- Pressing `f` with the mouse in the middle of the graph area will do a full X-axis zoom.
- Pressing `f` with the mouse on the left of the Y axis will do a full Y-axis zoom.
- Pressing `Left/Right` or `Up/Down` arrow keys while the mouse is inside a graph will move the waveforms to the left/right or zoom in/zoom out respectively.
- Pressing `Left/Right` arrow keys while the mouse is on the left of the Y-axis will zoom in/zoom out in the Y direction.
- Pressing the `left` mouse button while the pointer is in the center of the graph will move the waves left or right following the pointer X movement.
- Pressing the `left` mouse button while the pointer is on the left of the Y-axis will move the waves high or low following the pointer Y movement.
- pressing `A` and/or `B` will show a horizontal cursor. The difference between the `A` and the `B` cursor is shown.
- pressing `a` and/or `b` will show a vertical cursor. The sweep variable difference between the `a` and the `b` cursor is shown and the values of all signals at the X position of the `a` cursor is shown.
- Double clicking the `left` mouse button with the pointer above a wave label will allow to change its color.
- Pressing the `right` mouse button with the pointer above a wave label will show it in bold.
- Double clicking the `left` mouse button with the pointer in the middle of the graph will show a configuration dialog box, where you can change many graph parameters.
- Pressing the `right` mouse button in the graph area and dragging some distance in the X direction will zoom in the waveforms to that X range.
- Pressing the `right` mouse button to the left of the Y axis and dragging some distance in the Y direction will zoom in the waveforms to that Y range.

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:

- `?` Conditional expression: X cond Y ? --> return X if cond = 1 else Y

2 argument operators:

- `+` Addition
- `-` Subtraction
- `*` Multiplication
- `/` Division
- `<` Lower than
- `>` Greater than
- `==` Equal
- `!=` Not equal
- `<=` Lower or equal
- `>=` Greater or equal
- `==` Equal
- `==` Equal
- `**` Exponentiation
- `max()` Take the maximum of the two operators
- `min()` Take the minimum of the two operators
- `exch()` Exchange top 2 operands on stack
- `ravg()` Running average of over a specified time window
- `del()` Delete waveform by specified quantity on the X-axis
- `re()` Return real part of complex number specified as magnitude and phase (in deg)
- `im()` Return imaginary part of complex number specified as magnitude and phase (in deg)

1 argument operators:

- `sin()` Trig. sin function
- `cos()` Trig. cos function
- `tan()` Trig. tan function
- `sinh()` Hyp. sin function
- `cosh()` Hyp. cos function
- `tanh()` Hyp. tan function
- `asinh()` Inv hyp. sin function
- `acosh()` Inv hyp. cos function
- `atanh()` Inv hyp. tan function
- `asin()` Inverse trig. sin function
- `acos()` Inverse trig. cos function
- `atan()` Inverse trig. tan function
- `cph()` Continuous phase. Instead of [-180, +180] discontinuities make phase continuous
- `sqrt()` Square root
- `sgn()` Sign
- `abs()` Absolute value
- `exp()` Base-e Exponentiation
- `ln()` Base-e logarithm
- `log10()` Base 10 logarithm
- `idx()` point number (0, 1, 2, ...) in vector
- `db20()` Value in deciBel (20 * log10(n))
- `avg()` Average
- `prev()` Delay waveform by one point (at any x-axis position take the previous value)
- `deriv()` Derivative w.r.t. graph sweep variable
- `deriv0()` Derivative w.r.t. simulation (index 0) sweep variable
- `integ()` Integration
- `dup()` Duplicate last element on stack

### 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`.