Menu: Processes --> Netlist

The netlister creates a list of nets by analysing the schematic (the area inside the page border (see the workspace) ).  It can also be used to highlight wires associated with the netlist by double clicking in the netlist window (on the netlist data).  A flashing highlight in the schematic is shown - useful for checking that the schematic connects wires to the correct symbol pins.

 Status

The top panel shows the status of netlisting and the current actions being performed.

Netlist


The center panel shows the netlist output data.  Double clicking in this window will highlight the schematic wires (for each netlist).

You can also click the Part to decal (pcb footprint) mapping data lower down in this list starting from the text
     ; # mapping

Error panel 

The  error panel is not displayed unless an error occurs - to see it disconnect a wire from a pin and re-netlist.

If an error occurs a further panel is displayed showing the error data.  You can also click in this window to display the error on the schematic.

The two extra control sets are for more advanced use:

        "highlights" and "lock nets for pcb"

Advanced: Highlights

To review areas of the scheamtic clicking "accumulate highlights" will keep any highlights on the screen.  i.e. if you click a netlist it will hightlight the complete net in the schematic.  If "accumulate highlights" is also set then clicking another net will add a new highlight keeping the original.

This is useful if you want to review a set of nets.

Advanced: Lock Nets for pcb

After "Enable" is clicked repeat the netlist action by hitting "Netlist".  When you do this netnames are added to the schematic on the specified layer (here layer 7) for each unnamed net.

When you create a PCB it is useful to always use the same netnames because it is easier to identify the same net in the schematic and pcb tool.  Lock nets for pcb does this by adding netnames automatically and once they are added the connections will always adopt that netname.  

Note the netnames added automatically are exactly the same asnetnames added  manualy (they just use a smaller font size (which you can also change manually) so you can go and edit them (just remember to enable layer 7 as selectable and visible in the layer control dialog).

Note: Hitting Rem - removes the added netnames

Netlist schematic example

A net is a text description of the connections in the circuit e.g.:


Netlist example output

For the schematic above its netlist is :

 NET_ALPHA R1.1 R2.2 R3.1  ;( a single net)

; # mapping

R1    RES04
R2    RES04
R3    RES04

This describes the net (that has been labeled NET_ALPHA in the schematic) as connecting three components R1, R2 and R3 at pin 1 of R1 and pin 2 of R2 and pin 1 of R3.  Note that wires that are not given a net name are automatically assigned a unique net name during netlisting.

The mapping uses 'Decal' attribute data to define what footprint the part has.

Actions performed by the netlister

As well as generating the netlist the netlister checks the schematic for errors:

Checking pins
This checks that all pins in the schematic have either a wire connection or overlap another pin.  Wires do not have to be used to connect pins - it is sufficient for the pins themselves to overlap - can save space and effort in drawing schematics.

Checking for duplicate parts.
Ensures that there are no symbols with the same part Id.

Scanning nets.
Analysis the netnames and wires to generate the netlist information.

Processing overlapping pins.
Adds the overlapping pins to the netlist information


Processing power pins.
Adds pins defined as global parts generating their netlist data (see options  (Global parts) )

Merging and processing net data.
Merges data - can have multiple nets named the same when using netnames to label unconnected wires in the schematic, or when using multiple power pins.  Their data is merged into one net i.e. when using a power pins such as VOLT_BAR all the power pins having the same value define the same net i.e. all symbols connected to 5V (say) will all connect to the same 5V net. (see options  (Global parts)).

Detecting Single pin nets
If there is only one pin connected to a net then an error is indicated as usually this is an error, however the netlist is still generated as there are cases where this is not an error e.g. an aerial.

Detecting multiple netnames
When netnames are used to label wires all wires must have the same netname - if this is not true then an error is shown (see netnames).

Error display
As well as displaying the error in the netlister window the error is also circled within the schematic.  Holding the mouse over the error in the schematic will pop up data about the error.  To remove all errors from the schematic either use the edit menu control (see the  edit menu) or correct the errors and re-netlist.

An example netlist

0V R3.1 R4.1
9V R1.2 R2.2
BASE C1.1 R1.1 R3.2 TR2.2
NET_1 C1.2 IP1.1
NET_2 C2.1 OP1.1
NET_3 C2.2 R2.1 TR2.1
NET_4 R4.2 TR2.3

; # mapping

C1    CAP02
IP1   ""
OP1   ""
C2    CAP02
R1    RES04
R2    RES04
R3    RES04
R4    RES04
TR2   TO92


Note: The mapping part of the netlist defines the Decal (or footprint) of the part.  This information is useful for another tool e.g. pcb layout.  The decal defines the shape of the pcb footprint for the component.