- 11 - LibEdit : Complements
11.1
- Overview
11.2
- Positioning the anchor
11.3
- Alias
11.4
- Fields:
11.5
- Component documentation
- 11.5.1 - Keywords
-
11.5.2 - Component documentation (Doc)
-
11.5.3 - Associated documentation file (DocFileName)
-
11.5.4 - Footprint filtering for CVPCB
11.6
- Symbol library
- 11.6.1 - Export/Create a symbol
-
11.6.2 - Import a symbol
11 - LibEdit
: Complements
11.1 - Overview
- A component consist of several elements :
-
- Its graphic representation (geometrical shapes, texts).
-
- Pins.
- Fields, or associated texts, used by the post processors: netlist,
components list…
- Two fields are to be initialized : reference and value.
The
name of the design associated with the component, and the name of
the associated footprint, the other fields are the free fields, they
can generally remain empty, and could be filled during schematic
capture.-
However, managing the documentation associated with any component
facilitates the research, use and maintenance of the libraries.
-
The associated documentation consists of :
-
- A line of comment.
-
- A line of key words such as TTL CMOS NAND2…, separated by
spaces
-
- An attached file name (for example an application note, a pdf
file…). The default directory for attached files is
kicad/library/Doc.
-
- The key words allow you to selectively search for a component
according to varying selection criteria.
-
Comment and key words are displayed in various menus, and
particularly when you select a component in a library.
-
The component also has an anchoring point. A rotation or a mirror is
made relatively to this anchor point, and during a placement, this
point is used as a reference position. It is thus useful to position
this anchor accurately.
-
A component can also have aliases, i.e. equivalent names. This
allows you to considerably reduce the number of components that need
to be created (for example, a 74LS00 can have aliases such as 74000,
74HC00, 74HCT00…).
-
Finally, the components are distributed in libraries (classified by
topics, or manufacturer...), in order to facilitate their
management.
11.2 - Positioning
the anchor
- The anchor is at the co-ordinates 0,0 shown by the blue axes
displayed on the screen :
-

-
The anchor can be repositioned as follows :
-
Select the tool
and then click on the new desired anchor position. The drawing will
be automatically re-centered on this new anchor point.
11.3 - Alias
- An alias is another name corresponding to the same component in
the library.
-
Components with similar pinout and representation can then be
represented by only one component, having several aliases (ex: 7400
with alias 74LS00, 74HC00, 74LS37. ).
-
The use of aliases allows you to build complete libraries much more
quickly. In addition these libraries, being much more compact, are
loaded more quickly.
-
To modify the list of aliases, you have to select the main editing
window (tool
)
and select the Alias folder :

-
- You can thus add or remove the desired alias.
-
The current alias cannot obviously be removed since it is edited.
-
To remove all aliases, you have firstly to select the root component
(first component in the alias list in the window of selection of the
main toolbar).
11.4 - Fields:
- There are 4 special fields (texts attached to the component), et
8 user fields
-

-
- Special fields:
-
Reference
-
Value: It is the component name in library, and the default value
field in schematic.
-
Footprint : footprint name used for the board. Not veru usefull when
using CVPCB to setup the footprint list.
-
Sheet: reserved (not used at this time).
11.5 - Component
documentation
- To edit documentation information, it is necessary to call the
main editing window of the component (tool
)
and to select the Doc. Folder :-

-
- Caution:
-
Be sure to select the right alias, or the root component, because
this documentation is the only characteristic which differs between
aliases.
-
The "Copy Doc" button allows you to copy the documentation
information from the root component towards the currently edited
alias.
11.5.1 - Keywords
- The key words allow you to search in a selective way for a
component according to specific selection criteria (function,
technological family.)
-
The EESchema research tool isn't case sensitive.
-
The most current key words used in the libraries are :
-
CMOS TTL for the logic families
-
AND2 NOR3 XOR2 INV… for the gates (AND2 = 2 inputs AND gate,
NOR3 = 3 inputs NOR gate).
-
JKFF DFF… for JK or D flip-flop.
-
ADC, DAC, MUX…
-
OpenCol for the gates with open collector output.
Thus if in the
schematic capture software, you search the component: ( note the "="
at the beginning of the command ) =NAND2 OpenCol EESchema will
display the list of components having these 2 key words.
11.5.2 - Component
documentation (Doc)
- The line of comment (and key words) is displayed in various
menus, particularly when you select a component in the displayed
components list of a library and in the ViewLib menu.
-
If this Doc. file exists, it is also accessible in the schematic
capture software, in the popup menu displayed by a right-click on a
component.
11.5.3 - Associated
documentation file (DocFileName)
- Indicates an attached file (documentation, application
schematic…) available ( pdf file,schematic diagram…).
11.5.4 - Footprint
filtering for CVPCB
- One can enter a list of allowed footprints for the component.
-
This list acts as a filter used by CVPCB to display the allowed
footprints only.
-
A void list does not filter anything..

-
Wild cards are allowed.
-
S014* allows CVPCB to show all the footprints with a name
starting by SO14
-
For a resistor, R? shows all the footprints with a 2 letters
name starting by R.
-
Here are samples: with and without filtering

|
With filtering |

|
Without filtering |
11.6 - Symbol
library
- You can easily compile a graphic symbols library file containing
frequently used symbols .This can be used for the creation of
components (triangles, the shape of AND, OR, Exclusive OR gates…),
for saving and subsequent re-use.
-
These files are stored by default in the library's directory and
have a .sym extension.
-
The symbols are not gathered in libraries like the components
because they are generally not very numerous.
11.6.1 - Export/Create
a symbol
- A component can be exported as a symbol with the tool

-
You generally create only one graphic, also it will be a good idea
to delete all pins, if they exist.
11.6.2 - Import
a symbol
- That allows you to add graphics to a component you are editing.
-
A symbol is imported with the tool

-
Imported graphics are added as such as it was created in existing
graphics.
-