The following information may have errors; It is not permissible to be read by anyone who has ever met a lawyer. Use is confined to Engineers with more than 370 course hours of electronic engineering for theoretical studies. All content entered becomes and is (C)2007 Transtronics, Inc. the property of Transtronics, Inc. Rest assured that your contributions won't be sold and will be publicly available.
ph +1(785) 841 3089 Email inform@xtronics

From Transwiki

[edit] eeschema

[edit] Related kicad pages

• EE CAD Terminology
• kicad navigator or main kicad page
• eeschema - the schematic editor
• cvpcb - the component to module (AKA foot-print) editor
• pcbnew - the PCB layout program
• Gerbview - the Gerber file viewer

[edit] eschema

After you run through the tutorial - the next thing to do is learn how the libraries work. Libraries are processed with the subprogram called libedit.

[edit] libedit

If you are learning to use kicad, it is important to realize at step one that you will need to be able to make your own library parts (I can' think of a project where it wouldn't be true). The first thing you need to do is understand how the library parts are created, modified and extended. Libedit is where eeschema's library files (.lib) are edited. Once a part is edited you need to save it twice - into the current RAM and again to the library (not sure of the why for this?).

[edit] Managing Libraries

There are quite a few libraries that come with kicad and the temptation is use them just as they are, but the best practice is to create your own library and copy the ones you want to use over. Then if you make changes or adjustments you won't lose them the next time you update the software.

[edit] Change name of part in library

In libedit select part to rename, Select edit part properties and select the fields tab. In the "Field to edit" section, choose the "Value/Chip Name" radio button. While the "Value" radio button is selected, edit the "Field Text" to the new part name. Save the library. Select the delete icon and delete the original part name.

[edit] Create New Parts Library

From in EESchema select click-on go_to_library-editor" icon. Then select "New Component" icon ... go through the process of creating a part or open an existing one it by clicking on the 'Select a component to edit' icon.

Once you've have a part, use the "Create a new library and save current part into" icon. Then select a filename (ends in '.lib').

After saving - close out libedit. Next, form in EESchema add the new library to library list. You do this in "Preferences/Libs_and_Dir > ADD (button)" - browse and find the library you just created and it will be added to the selection list.

[edit] Copy part between libraries

From in EESchema select click-on go_to_library-editor" icon. From within libedit click on the 'Select the working library' icon - select the lib you want to copy from and then click on the 'Select a component to edit' icon and select the part you want to copy.

Now, click on the 'Select the working library' icon again and then the 'save current loaded library on disk' icon.

[edit] Define Field names for parts Library

Once you understand how the library works, the next thing you should do is to decide on a default set of fields that you want associated with your parts - this allows you to have the information where it is needed and helps you generate useful BOMs.

There are only a couple of field names (of course the field itself is editable) that can't be changed. These are Ref, Value/Chip Name, Footprint, and Sheet,

Ref 

this is the reference number - its default value will be the reference prefix - R for resistor C for Cap etc

Value/Chip Name; (the part-name ie 2N2222 (the default name here is confusing!!)),

Footprint

the name of the circuit board decal that the part points to. If the part can have more than one foot print leave it blank and use Footprint filtering to enter a list of possible footprint.

Sheet

(Should be subsheet? - the name of the sub sheet the part is on??

The rest of the fields are user fields that default to field1, field2,...field8 and can be changed to anything you want.

I recommend creating a part called 'template' that has the fields you normally use and save it. Then when you create a new part open this 'template-part' and edit it into the new part. I suggest the following fields to use:

• Value (not to be confused with the Value/Chip Name) This field can be used with resistors, capacitors etc and have the resistance value.

• Description - a brief string that describes the part ie 256K Eprom, 1/4 watt resistor, edge connector.

• Manu1 - First manufacturer

• manu1# - First manufacturer's part number

• Manu2 - First manufacturer

• manu2# - First manufacturer's part number

• Vendors - Who distributes this part

• Pricing - I put info like $.002 in 10,000s

[edit] Part Properties

While in lib edit you can click on the 'Edit component Properties icon to bring up a tabbed dialog box. This lets you change the details of the component.

[edit] Options Tab

As Convert 

This is for logic gates - the convert is the De'Morgan's equivalent of the main part.

Show Pin Num and Show Pin Name

Makes Pin names and numbers visible. Normally checked for chips, but would be cleared for resistors and diodes.

Pin Name inside

Normally checked - it is the norm for chips.

Number of Units

How many op-amps in the quad package? 5 - 4 op-amps + one power part

Skew

Power Symbol

Parts are locked

[edit] Doc Tab

Doc 

A text string that is displayed in various menus in displayed lists of libraries.

keywords 

key words allow you to search in a selective way for a component according to specific selection criteria

(function, technological family.)

DocFileName 

Points to the documentation file for the component - a PDF or schematic.

Copy Doc

Browse DocFiles

[edit] Alias Tab

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. ).

Add

Add a new Alias

Delete and Delete all

Remove one or all Alias

[edit] Fields Tab

Field to Edit

Click radio button to work with a selected field

Show Text

Makes the selected field's text visible when in eescheema

Vertical

Select to rotate the text side ways.

Field Name 

name of the field - see #Define Field names for parts Library

Field Text 

The text the Field holds.

Size - Posx - PosY

How large the text and what offset the text is at from part the part origin or anchor point

Horizontal and vertical Justify 

Sets the justification of the text - left, centered, or right.

[edit] Footprint Filter Tab

Footprints

Enter a list of allowed footprints for the component. This list acts as a filter used by CVPCB to display the allowed footprints only. 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

Add

Delete and Delete all 

[edit] Schematic Parts creation

My way is to always start with my template part (you could have several templates made from the first one.) So instead of selecting the New component' icon use the select component to edit icon and change the Value/Chip Name field and save the part. Then start editing.

• Saving to current loaded (RAM) library updates schematic. Don't forget to save to the Library
• Pin names with an over-bar (active low) can be made by starting the name with a '`' tilde..
• Skew setting is the distance between text and pin end.
• Over-lines for logic notation can be accomplished in pin names using the tilde ('~") character. For example:
  • Enter read/~write to display read/write or ~write~/read would appear as write/read

[edit] libbrowse

Associate schematic decal pins with footprint pins?

[edit] ERC

Electrical Rule Check helps check your schematic for errors.

[edit] eschema How-to do things

[edit] Update a part with one newly modified in the library

Make sure you save both to the lib and RAM before leaving libedit

[edit] Change part value

Do not change the value/partname field - it is actually the part name - you will need to select edit part and create a custom value field.

[edit] Placing multiple components of the same type

Select the component, R-click and from the pop-up menu, "copy-component". If you need to duplicate a block of components, hold shift, L-click and drag a box around them, drag and release.

[edit] Copy of a block of schematic from one sheet to another

Select the block with the mouse, right-click and select "Save block" Then go to the other sheet and click the "Paste" button in the tool-bar.

[edit] Copying from project to project

You can do this by adding the old schematic to the new as a hierarchical sheet and the copying between them.

1. Copy the old schematic file to the same directory as your new schematic file.
2. Select the "Add hierarchical Symbol" icon (Right tool bar) and place one on the new schematic.
3. Enter the file name of the old schematic you copied into the directory including the file name extension. Leave the sheet name blank.
4. Open the old schematic via the "schematic hierarchy navigator" icon (Top tool bar) or double click on the symbol.
5. Select the block you want to copy and pick "Save Block" from the context menu.
6. Open the new schematic via the "schematic hierarchy navigator" icon (Top tool bar).
7. Select the "Paste" icon and paste the block in the new schematic.
8. Repeat as required.
9. Delete the old schematics hierarchical Symbol from the new schematic.
10. Delete the old schematic file if you want.

[edit] Printing to a web viewable file

A better solution than postscript printing is to use Plot/Plot SVG command to write scheme in SVG file format.

• • The only drawback is width of the lines - there is a script that only changes stroke-width:1 to stroke-width:10 in SVG file and it can be found at http://www.japina.eu/blog

[edit] Block move

Proceed as follows:

1. Hold down Ctrl
2. Press and hold down the left mouse button to begin selecting
3. You can release Ctrl any time from now
4. Move to the opposite corner of the selection box and release the left mouse button
5. Move the items to the desired place and left-click to put them there

• • If anything goes wrong, right-click and select "Cancel block".

[edit] Notes

• For multi-part components with more than one component type, do not forget to check (in library editor) the "Parts are Locked" option for these components. With this option, Eeschema does not change the part selection when annotates the schematic.
• The locate dialog has a search for markers - these markers refer to those produced by ERC.

[edit] The Files of kicad

• .pro Project file Contains lib selections, default directory and other details about the project. It maintains a number of parameters relating to project management (such as the filename of the principal schematic, list of libraries used in the schematics and PCBs).
• .sch Schematic file
• .lib eeschema library file - also the file type that is exported and imported in libedit
• .bac backup of a .lib file
• .dcm - Items from Libedit - properties/Doc-tab Document file name, keywords for lib files (name.lib and name.mdc go together (why not the same file>?))
• .bck backup of a .dcm file
• .sym - these are symbols without parts (gates i.e NAND, NOR, opamp, )
• .brd PCB file
• .net Netlist file.
• .mod - footprints
• .mdc - associated documentation file (name.mod and name.mdc go together (why not the same file>?))
• .emp - export of module
• .equ - maps part-name to footprint
• .stf - back annotation file - fills in the footprint field in eeschema from what is selected in cvpcb
• .rpt created by File/export /module report
• .cmp auxiliary component assignment file - a file that associates the Reference, part-name and footprint - Generated by CVPCB
• .wings 3d part model file
• .wrl VRML model
• project-cmp.pos create a Module Position File with Postprocess->Create Modules Pos (this is the component side)
• project-copper.pos (As above but this is the solder side)
• project.cache.lib Cache file of the libraries used in the schematic (backup of the components used)

[edit] Notes

[edit] Power Ports

Power ports are the ground and power symbols. As of 0.0.20080825c they must be in a library named 'power.lib'. If you try to create your own power lib under a different name you will have problems.

[edit] Power flag Behavior

Only the pin name is used. Invisible pins which have the Power In or Power Out electrical contact are automatically connected. Because your GND_EARTH symbol has a pin named GND, this pin is connected to the GND net.

For connection, the name of the symbol is not used (From this point of view, if is only a comment). A GND_EARTH symbol must be build with a single pin named GND_EARTH. (See Eeschema doc, chapter 10.8)

In order to avoid problems, the flag "Power Symbol" must be set (In libedit, Part Properties). When this flag is set: - One cannot edit the symbol name in eeschema. - The symbol is automatically reannotated when an ERC or a netliste is made.

Advantage

You can easily create power symbols with the shape you like, because it is a component, like others components.

Drawback

You cannot create a new power symbol only by editing its name: you must create a new symbol (i.e. a new component), with the shape you want, an a pin which have the same name as the symbol name.