PREV UP NEXT

# XSCHEM PROPERTIES

Properties are text strings that are associated to XSCHEM objects. All graphic primitives support properties.

- Wires
- Lines
- Rectangles
- Texts
- Symbols

Consider for example the `res.sym` symbol (you may open it with the `Open` menu item) if you click inside one of the red pins and press the 'edit property' bindkey `'q'` a dialog box shows the property string associated with the selected pin:

The `name=p dir=inout` property string tells that the selected pin name is `'p'`, this will be the symbol positive pin name in the produced netlist. The property string also defines a `dir` attribute with value `inout`. This tells XSCHEM that electrically this is an input/output pin. This is important when producing VHDL/verilog netlists. The second (bottom) pin property string is `name=m dir=inout` and this defines the negative pin. The text primitives also have properties. For texts the property string may be used to specify font and the layer to use for displaying text.

### GLOBAL PROPERTIES

If you click outside of any displayed graphics in XSCHEM the selection set will be cleared. Clicking the edit property `'q'` key when nothing is selected will display the global property string of the schematic (.sch) or symbol window (.sym).

There is actually one different global property string defined for any available netlisting modes, so if XCHEM is set to produce SPICE netlists the SPICE global property string is displayed.

So, in addition to properties associated to graphical objects and symbols we also have properties associated to schematic (.sch) and symbol files (.sym)

The `format` attribute defines the format of the SPICE netlist. The SPICE netlist element line starts with the symbol name (in this case a resistor so 'rxxxxx'), the list of pins, the resistor value and a multiplicity factor (m).
`@pinlist` will resolve to the parent nets attached to the resistor nodes, in the order they appear in the symbol (in this example; first node = 'p', second node = 'm').
We will return on component instantiation later, but for now, considering the following picture:

the `@pinlist` for the `r1` component will expand to `POS NEG`.
`@value` resolves to the resistor value assigned in component instantiation. The `template` attribute defines default values if component instantiation does not define values for them.
If you want to add a pin to an existing symbol you may copy one of these. Select a pin, press the copy `'c'` bindkey and place a new copy of it somewhere.

After copying the pin you may change its properties, for example you will change its property string to something like: `name=body dir=in` (just as an example).
Note that pins in symbols are nothing more than rectangles drawn with the `pin` layer; instead of copying an existing one you may create it from scratch, select the pin layer from the `Layers` menu, point the mouse where you want to place the pin, press the `'r'` bindkey and drag the mouse to the desired pin size. There is no inherent limit or assumption on pin sizes, you are allowed to create any rectangular/square sizes. After placing the rectangle you must create a property string by selecting it and pressing the `'q'` bindkey. An empty string is shown in the dialog. Add a valid string as explained and you are all done.

### PIN ORDERING

An important aspect for symbols is the order of the pins when producing the netlist. There are some rules in the order for example in SPICE netlist syntax; for example a Bipolar transistor has 3 pins and should be in a specific order (collector, base, emitter). When done placing pins on a newly created symbol you can specify the order by selecting the one that must be the first in the netlist and hitting the `'<shift>S'` bindkey; set the number to zero; this will make the selected pin the first one. Next, select the second pin and again hit `'<shift>S'`, set its number to 1 and so on. By doing so you have defined a specific pin ordering of the symbol.