:experimental: [[assigning-footprints]] == Assigning Footprints Before routing a PCB, footprints need to be selected for every component that will be assembled on the board. Footprints define the copper connections between physical components and the routed traces on a circuit board. Some symbols come with footprints pre-assigned, but for many symbols there are multiple possible footprints, so the user needs to select the appropriate one. KiCad offers several ways to assign footprints: * Symbol Properties ** Symbol Properties Dialog ** Symbol Fields Table * While placing symbols * Footprint Assignment Tool Each method will be explained below. Which to use is a matter of preference; one method may be more convenient depending on the situation. All of these methods are equivalent in that they store the name of the selected footprint in the symbol's `Footprint` field. NOTE: The Footprint Library Table needs to be configured before footprints can be assigned. For information on configuring the Footprint Library Table, please see the xref:../pcbnew/pcbnew.adoc#managing-footprint-libraries[PCB Editor manual]. [[assigning-footprints-in-symbol-properties]] === Assigning Footprints in Symbol Properties A symbol's `Footprint` field can be edited directly in the symbol's Properties window. image::images/eeschema_symbol_properties_footprint.png[scaledwidth="70%", alt="Assigning footprint in Symbol Properties"] Clicking the image:images/icons/small_library_16.png[library icon] button in the `Footprint` field opens the Footprint Chooser, which shows the available footprints sorted by footprint libraries. The Footprint Chooser filters footprints by name, description, and keywords, as well as any fields that are shown as columns, according to what you type into the search field. `*` and `?` wildcards are available. The footprint search behaves the same as in the <>. If the symbol defines any <>, the **apply footprint filters** option can be used to hide footprints that don't match those filters. If the **filter by pin count** option is selected, only footprints that match the symbol's pincount will be listed. You can choose to sort search results alphabetically or by best match by clicking on the image:images/icons/small_sort_desc_16.png[sort button] button. Single clicking a footprint name selects the footprint and displays it in the preview pane on the right. You can switch between a 2D and 3D preview of the footprint by clicking the image:images/icons/module_16.png[2D component icon] and image:images/icons/three_d_16.png[3D component icon] buttons. Double clicking on a footprint closes the chooser and sets the symbol's `Footprint` field to the selected footprint. image::images/footprint_chooser.png[scaledwidth="80%", alt="Selecting a footprint in Footprint Chooser"] [[assigning-footprints-with-the-symbol-fields-table]] ==== Assigning Footprints with the Symbol Fields Table Rather than editing the properties of each symbol individually, the Symbol Fields Table can be used to view and edit the properties of all symbols in the design in one place. This includes assigning footprints by editing the `Footprint` field of each symbol. The Symbol Fields Table is accessed with **Tools** -> **Edit Symbol Fields...**, or with the image:images/icons/spreadsheet_24.png[Symbol Fields Table Icon] button on the top toolbar. The `Footprint` field behaves the same here as in the Symbol Properties window: it can be edited directly, or footprints can be selected visually with the Footprint Library Browser. image::images/eeschema_symbol_fields_table_footprint.png[scaledwidth="90%", alt="Bulk editing footprint assignments with the Symbol Fields Table"] For more information on the Symbol Fields Table, see the <>. [[assigning-footprints-while-placing-symbols]] === Assigning Footprints While Placing Symbols Footprints can be assigned to symbols when the symbol is first added to the schematic. Some symbols are defined with a default footprint. These symbols will have this footprint preassigned when they are added to the schematic. If a symbol has a default footprint, the footprint will be graphically previewed in the symbol chooser dialog when the symbol is selected. For symbols without a default symbol defined, the footprint dropdown will say "No default footprint", and the footprint preview canvas will say "No footprint specified". image::images/eeschema_add_symbol_default_footprint.png[Default footprint in Add Symbol dialog] Symbols can have footprint filters that specify which footprints are appropriate to use with that symbol. If footprint filters are defined for the selected symbol, all footprints that match the footprint filters will appear as options in the footprint dropdown. The selected footprint will be displayed in the preview canvas and will be assigned to the symbol when the symbol is added to the schematic. NOTE: Footprint options will not appear in the footprint dropdown unless the footprint libraries are loaded. Footprint libraries are loaded the first time the Footprint Editor or Footprint Library Browser are opened in a session. For more information on footprint filters, see the <>. [[footprint-assignment-tool]] === Assigning Footprints with the Footprint Assignment Tool The Footprint Assignment Tool allows you to associate symbols in your schematic to footprints used when laying out the printed circuit board. It provides footprint list filtering, footprint viewing, and 3D component model viewing to help ensure the correct footprint is associated with each component. Components can be assigned to their corresponding footprints manually or automatically by creating equivalence files (.equ files). Equivalence files are lookup tables associating each component with its footprint. Run the tool with **Tools** -> **Assign Footprints...**, or by clicking the image:images/icons/icon_cvpcb_24_24.png[Footprint Assignment Tool icon] icon in the top toolbar. ==== Footprint Assignment Tool Overview The image below shows the main window of the Footprint Assignment Tool. image::images/en/cvpcb_main_window.png[scaledwidth="90%", alt="The main window of the Footprint Assignment Tool"] * The left pane contains the list of available footprint libraries associated with the project. * The center pane contains the list of symbols in the schematic. * The right pane contains the list of available footprints loaded from the project footprint libraries. * The bottom pane describes the filters that have been applied to the footprint list and prints information about the footprint selected in the rightmost pane. The top toolbar contains the following commands: [width="80%",cols="10%,90%",] |======================================================================= |image:images/icons/save_24.png[] |Transfer the current footprint associations to the schematic. |image:images/icons/library_table_24.png[] |Edit the global and project footprint library tables. |image:images/icons/icon_footprint_browser_24.png[] |View the selected footprint in the footprint viewer. |image:images/icons/left_24.png[] |Select the previous symbol without a footprint association. |image:images/icons/right_24.png[] |Select the next symbol without a footprint association. |image:images/icons/undo_24.png[] | Undo last edit. |image:images/icons/redo_24.png[] | Redo last edit. |image:images/icons/auto_associate_24.png[] |Perform automatic footprint association using an equivalence file. |image:images/icons/delete_association_24.png[] |Delete all footprint assignments. |image:images/icons/module_filtered_list_24.png[] |Filter footprint list by footprint filters defined in the selected symbol. |image:images/icons/module_pin_filtered_list_24.png[] |Filter footprint list by pin count of the selected symbol. |image:images/icons/module_library_list_24.png[] |Filter footprint list by selected library. |======================================================================= The following table lists the keyboard commands for the Footprint Assignment Tool: [width="80%",cols="15%,85%",] |======================================================================= |Right Arrow / Tab|Activate the pane to the right of the currently activated pane. Wrap around to the first pane if the last pane is currently activated. |Left Arrow |Activate the pane to the left of the currently activated pane. Wrap around to the last pane if the first pane is currently activated. |Up Arrow |Select the previous item of the currently selected list. |Down Arrow |Select the next item of the currently selected list. |Page Up |Select the item one full page upwards of the currently selected item. |Page Down |Select the item one full page downwards of the currently selected item. |Home |Select the first item of the currently selected list. |End |Select the last item of the currently selected list. |======================================================================= ==== Manually Assigning Footprints with the Footprint Assignment Tool To manually associate a footprint with a component, first select a component in the component (middle) pane. Then select a footprint in the footprint (right) pane by double-clicking on the name of the desired footprint. The footprint will be assigned to the selected component, and the next component without an assigned footprint is automatically selected. NOTE: If no footprints appear in the footprint pane, check that the <> are correctly applied. When all components have footprints assigned to them, click the **OK** button to save the assignments and exit the tool. Alternatively, click **Cancel** to discard the updated assignments, or **Apply, Save Schematic & Continue** to save the new assignments without exiting the tool. [[filtering-the-footprint-list]] ===== Filtering the Footprint List There are four filtering options which restrict which footprints are displayed in the footprint pane. The filtering options are enabled and disabled with three buttons and a textbox in the top toolbar. * image:images/icons/module_filtered_list_24.png[]: Activate <>. For example, an opamp symbol might define filters that show only SOIC and DIP footprints. * image:images/icons/module_pin_filtered_list_24.png[]: Only show footprints that match the selected symbol's pin count. * image:images/icons/module_library_list_24.png[]: Only show footprints from the library selected in the left pane. * Entering text in the textbox hides footprints that do not match the text. This filter is disabled when the box is empty. When all filters are disabled, the full footprint list is shown. The applied filters are described in the bottom pane of the window, along with the number of footprints that meet the selected filters. For example, when the symbol's footprint filters and pin count filters are enabled, the bottom pane prints the footprint filters and pin count: image::images/en/filter_details.png[scaledwidth="80%", alt="Filter details when symbol footprint filters and pin count filter are enabled"] Multiple filters can be used at once to help narrow down the list of possibly appropriate footprints in the footprint pane. The symbols in KiCad's standard library define footprint filters that are designed to be used in combination with the pin count filter. [[automatically-associating-footprints-to-components]] ==== Automatically Assigning Footprints with the Footprint Assignment Tool The Footprint Assignment Tool allows you to store footprint assignments in an external file and load the assignments later, even in a different project. This allows you to automatically associate symbols with the appropriate footprints. The external file is referred to as an equivalence file, and it stores a mapping of a symbol value to a corresponding footprint. Equivalence files typically use the `.equ` file extension. Equivalence files are plain text files with a simple syntax, and must be created by the user using a text editor. The syntax is described below. You can select which equivalence files to use by clicking **Preferences** -> **Manage Footprint Association Files** in the Footprint Assignment Tool. image::images/en/cvpcb_equivalence_files.png[Managing equivalence files] * Add new equivalence files by clicking the *Add* button. * Remove the selected equivalence file by clicking the *Remove* button. * Change the priority of equivalence files by clicking the *Move Up* and *Move Down* buttons. If a symbol's value is found in multiple equivalence files, the footprint from the last matching equivalence file will override earlier equivalence files. * Open the selected equivalence file by clicking the *Edit File* button. Relevant environment variables are shown at the bottom of the window. When the *Relative* path option is checked, these environment variables will automatically be used to make paths to selected equivalence files relative to the project or footprint libraries. Once the desired equivalence files have been loaded in the correct order, automatic footprint association can be performed by clicking the image:images/icons/auto_associate_24.png[Perform automatic footprint assignment icon] button in the top toolbar of the Footprint Assignment Tool. All symbols with a value found in a loaded equivalence file will have their footprints automatically assigned. However, symbols that already have footprints assigned will not be updated. [[equivalence-file-format]] ===== Equivalence File Format Equivalence files consist of one line for each symbol value. Each line has the following structure: `'' ':'` Each name/value must be surrounded by single quotes (`'`) and separated by one or more spaces. Lines starting with `#` are comments. For example, if you want all symbols with the value `LM4562` to be assigned the footprint `Package_SO:SOIC-8_3.9x4.9_P1.27mm`, the line in the equivalence file should be: `'LM4562' 'Package_SO:SOIC-8_3.9x4.9_P1.27mm'` Here is an example equivalence file: ---- #integrated circuits (smd): '74LV14' 'Package_SO:SOIC-14_3.9x8.7mm_P1.27mm' 'EL7242C' 'Package_SO:SOIC-8_3.9x4.9_P1.27mm' 'DS1302N' 'Package_SO:SOIC-8_3.9x4.9_P1.27mm' 'LM324N' 'Package_SO:SOIC-14_3.9x8.7mm_P1.27mm' 'LM358' 'Package_SO:SOIC-8_3.9x4.9_P1.27mm' 'LTC1878' 'Package_SO:MSOP-8_3x3mm_P0.65mm' '24LC512I/SM' 'Package_SO:SOIC-8_3.9x4.9_P1.27mm' 'LM2903M' 'Package_SO:SOIC-8_3.9x4.9_P1.27mm' 'LT1129_SO8' 'Package_SO:SOIC-8_3.9x4.9_P1.27mm' 'LT1129CS8-3.3' 'Package_SO:SOIC-8_3.9x4.9_P1.27mm' 'LT1129CS8' 'Package_SO:SOIC-8_3.9x4.9_P1.27mm' 'LM358M' 'Package_SO:SOIC-8_3.9x4.9_P1.27mm' 'TL7702BID' 'Package_SO:SOIC-8_3.9x4.9_P1.27mm' 'TL7702BCD' 'Package_SO:SOIC-8_3.9x4.9_P1.27mm' 'U2270B' 'Package_SO:SOIC-16_3.9x9.9_P1.27mm' #regulators 'LP2985LV' 'Package_TO_SOT_SMD:SOT-23-5_HandSoldering' ---- ==== Viewing the Current Footprint The Footprint Assignment Tool contains a footprint viewer. Clicking the image:images/icons/icon_footprint_browser_24.png[footprint viewer icon] button in the top toolbar launches the footprint viewer and shows the selected footprint. image::images/en/footprint_view.png[scaledwidth="90%", alt="Viewing a footprint"] The top toolbar contains the following commands: [width="90%",cols="10%,90%",] |======================================================================= |image:images/icons/refresh_24.png[] |Refresh view |image:images/icons/zoom_in_24.png[] |Zoom in |image:images/icons/zoom_out_24.png[] |Zoom out |image:images/icons/zoom_fit_in_page_24.png[] |Zoom to fit drawing in display area |image:images/icons/shape_3d_24.png[] |Show 3D viewer |======================================================================= The left toolbar contains the following commands: [width="90%",cols="10%,90%",] |======================================================================= |image:images/icons/cursor_24.png[] |Use the select tool |image:images/icons/measurement_24.png[] |Interactively measure between two points |image:images/icons/grid_24.png[] |Display grid dots or lines |image:images/icons/polar_coord_24.png[] |Switch between polar and cartesian coordinate systems |image:images/icons/unit_inch_24.png[] |Use inches |image:images/icons/unit_mil_24.png[] |Display coordinates in mils (1/1000 of an inch) |image:images/icons/unit_mm_24.png[] |Display coordinates in millimeters |image:images/icons/cursor_shape_24.png[] |Toggle display of full-window crosshairs |image:images/icons/pad_number_24.png[] |Toggle between drawing pads in sketch or normal mode |image:images/icons/pad_sketch_24.png[] |Toggle between drawing pads in normal mode or outline mode |image:images/icons/text_sketch_24.png[] |Toggle between drawing text in normal mode or outline mode |image:images/icons/show_mod_edge_24.png[] |Toggle between drawing graphic lines in normal mode or outline mode |======================================================================= ===== Viewing the Current 3D Model Clicking the image:images/icons/shape_3d_24.png[3D Viewer icon] button opens the footprint in the 3D model viewer. NOTE: If a 3D model does not exist for the current footprint, only the footprint itself will be shown in the 3D Viewer. image::images/en/3d_window.png[scaledwidth="90%", alt="3D-Model view"] The 3D Viewer is described in the xref:../pcbnew/pcbnew.adoc#threed-viewer[PCB Editor manual].