4. Creating your circuit: schematic capture

4.1. Gschem attributes for spice netlisting

There are several ways that spice attributes may be associated with a component using gschem. The way you choose to do this depends upon many factors, including the type of component, and the size and format of the SPICE model.

4.2. Component attributes and meanings

The following attributes are meaningful for SPICE netlisting, and may be attached from within gschem:

• refdes: The reference designator of the component. Valid values depend upon the component type and are given in the appendix.

• value: For passives, this is the component value. For actives, this is the type (model no.) of the component (e.g. 2N3904, uA741). When a model for an active is instantiated separately from the component itself, the value attribute holds the name of the spice model.

• model: This holds a one line spice model for the component.

• file: This holds the name of a file. Typically, this is a file holding e.g. a SPICE .MODEL, .SUBCKT, or other SPICE code.

• model-name: This holds the name of the spice model referred to in a .MODEL or .SUBCKT statement. model-name is mainly used to identify the spice model name in the symbol spice-model-1.sym. Active components should call out this name in the device attribute to associate the component with its particular spice model or subcircuit.

• type: This specifies the type of component and is used by spice when interpreting the model parameters. Valid values depend upon the device being modeled.

4.3. refdes conventions

As a prerequisite to handling SPICE-related attributes, the SPICE netlister requires that all components must have a refdes attached to them. The refdes may be attached either by hand (which is laborious), or using the program refdes_renum included in the gEDA distribution.

Note that the first letter of the refdes must correspond to the appropriate letter for spice simulation. The refdes convention is given in the appendix.

4.4. Passives

4.5. Passives with additional attributes

Oftentimes, passive components have additional attributes attached to them for spice simulation. Examples of such attributes are temperature coefficients (for resistors) and initial conditions (for reactive components). These additional components may be incorporated into the SPICE file by simply attaching them to the component's model attribute. Specifically, the required attributes are:

• refdes: Correct component refdes.

• value: Numerical component value, as always.

• model: One line string holding additional parameters, formatted as a valid SPICE string.

This string is placed after the component value in the line generated by gnetlist. Therefore, it is important to format the string placed in the model line to be valid SPICE code. Otherwise, you will risk causing the SPICE simulator to barf.

4.6. Passives for semiconductor design

The values for resistors and capacitors are often given as dimensions in an ASIC design. SPICE takes from the technology library the typical value per square and calculates the actual value in Ohm or Farad by itself. Therefor the following attributes are required:

• refdes: The correct refdes for the component

• model-name: corresponds to the model in the technology library

• w, l: dimensions of the device

The technology library must be included with an .include line in the SPICE input file.

4.7. Transistors and diodes

Transistors and diodes are generally accompanied by a device-specific model. Each model attempts to capture the detailed nonlinear dynamics of its particular device; otherwise, SPICE simulation is pointless. The SPICE model may be either a short, one-line string of parameters, or a multi-line set of SPICE parameters. A typical one-line parameter string is a short list of parameters describing a small-signal diode. Typical multi-line models come from component vendors, who often provide models for their components in a text file. Since there are two broad formats of SPICE information, there are two approaches to incorporating these parameters into the schematic:

4.8. Actives -- integrated circuits

Integrated circuits are incorporated into the netlist similarly to transistors and diodes. As such, you may incorporate the spice information either as a one-line parameter string, or as a model file.

4.9. Independent sources

There are two independent sources: voltage sources and current sources. For incorporation into a SPICE netlist, they both work the same way. To incorporate an independent source into your SPICE netlist, do the following:

1. Place the independent source on your schematic. (Do Add -> Component -> spice -> <independent source name>.sym)

2. Double click on the block and add/edit the following attributes:

   • refdes: V? or I?

   • value: A one line string in SPICE format describing the source.

4.10. Dependent sources

There are four dependent sources:

This section remains TBD.

4.11. SPICE components

4.12. Handling hierarchical models

In SPICE modeling, there are often situations where you wish to create a schematic representation of some particular component as a .SUBCKT, and then embed that component's model in a higher level schematic. A common example might be as follows: You are doing a microwave simulation, and want to use a capacitor model which includes parasitic inductances and resistances, as well as the capacitance. Capacitor manufacturers often supply a printed schematic showing a circuit topology incorporating parasitics, and specify values for the parasitics. You would like to draw the capacitor model using gschem, netlist it to create a .SUBCKT, and then use the .SUBCKT to model capacitors in a higher lever schematic.

Since this kind of task is very common in SPICE simulation, gnet-spice-sdb now supports it (starting with rev 20030331). To create a lower level .SUBCKT and use it in a higher level schematic, do the following:

1. Draw the schematic of the lower level component (e.g. the capacitor + parasitics) using gschem.

2. On the lower level schematic, place a spice-subcircuit-LL block (spice-subcircuit-LL-1.sym). This alerts the netlister that the schematic is a Lower Level .SUBCKT. Attach the following attributes to the symbol:

   • model-name = cap_with_parasitics

   (Of course, “cap_with_parasitics” is the example we use here. Use your own model name in your schematic.) Upon netlisting, this schematic symbol will cause the netlist to insert “.SUBCKT cap_with_parasitics” into the first line of the netlist file.

3. On the lower level schematic, attach a spice-subcircuit-IO symbol (spice-subcircuit-IO-1.sym) to each IO net (i.e. connection to the upper level). Number the refdeses of the IO symbols in the same order as you would like the IO nets to be listed in the .SUBCKT line in the output file. (i.e. P1 = first, P2 = second, etc.)

4. When you are done with the lower level schematic, netlist it in the usual way. For example, if your schematic is called cap_with_parasitics.sch, netlist it by saying: gnetlist -g spice-sdb -o cap_with_parasitics.cir cap_with_parasitics.sch This will dump the SPICE netlist into the file called “cap_with_parasitics.cir”. Visually inspect the .cir file to make sure that netlisting worked correctly.

5. Next, create a symbol for the upper level schematic which will point to the .SUBCKT. Note that the symbol must have a refdes starting with the letter “X”. To ensure that this happens, do the following:

   1. Use gschem to draw the symbol. I usually draw a box around a model symbol to distinguish it from a normal component. Make any other annotations desired.

   2. In the symbol, make sure that the pins are ordered identically to the order in which you have placed the pins in the .SUBCKT. This is done by editing the symbol with a text editor and setting the pinseq attribute. The netlister will output the pins in the order determined by the pinseq attribute.

   3. Using a text editor, give the symbol a device attribute like “capacitor-model”. Do not assign the symbol one of the native device types listed in the appendix! The goal is to create a symbol whose refdes starts with “X”, and if the device is a recognized type, this will not happen.

   4. Using a text editor, give the symbol the refdefs attribute “X?”

6. Create the upper level schematic. Place your newly created symbol on the schematic as many times as required and wire up the schematic in the usual way.

7. To point your symbol to the lower level .SUBCKT, double click on the symbol and set the following attributes:

   • file = cap_with_parasitics.cir

   • model-name = cap_with_parasitics

   as well as any other attributes required (e.g. refdes).

8. Now netlist your upper level schematic the usual way. The contents of each .SUBCKT file is dumped into the main netlist. Inspect your netlist visually using a text editor to ensure that it is correct. It is a good idea to pay particular attention to the following:

   • Verify that the ordering of the nets connecting the upper level netlist to the lower level .SUBCKT is correct.

   • Make sure that the upper level model-name and the lower level model name (on the .SUBCKT declaration line) are the same.

Once the netlist is created, you may simulate your design using any SPICE simulator desired. Some simulators running on Linux are covered below.