Creating a PCB Footprint

Now reading version 23. For the latest, read: Creating a PCB Footprint for version 24

The area that the component occupies on the fabricated board is defined by the component footprint. A typical footprint includes pads and a component overlay, and can also include any other mechanical details required. In the example footprint below, most of the component outline is defined on a mechanical layer (the green lines) rather than the (yellow) overlay, because this component will be mounted so that it hangs over a cutout in the board.

The footprint defines the space the component occupies and provides the points of connection from the component pins/pads to the routing on the board. 
The footprint defines the space the component occupies and provides the points of connection from the component pins/pads to the routing on the board.

The component that is mounted on that footprint can be modeled using 3D Body objects. The 3D Body object is used as a container into which a generic MCAD format model can be imported, as shown in the image below.

A suitable MCAD model can be imported into a 3D Body object.
A suitable MCAD model can be imported into a 3D Body object.

Even with a rich set of resources providing ready-made PCB components (such as the Manufacturer Part Search panel), it is likely that at some point in your career you will need to create a custom PCB component. PCB component footprints are created in the PCB footprint editor using the same set of primitive objects available in the PCB editor. In addition to footprints, company logos, fabrication definitions, and other objects required during board design can also be saved as PCB components.

Creating a New PCB Footprint

Footprints can be created directly in your connected Workspace.

  1. Select File » New » Library from the main menus, then in the New Library dialog that opens, select Create Library Content » Footprint from the Workspace region of the dialog.

    Create a new Workspace Footprint using the New Library dialog
    Create a new Workspace Footprint using the New Library dialog

  2. In the Create New Item dialog that opens, enter the required information, make sure that the Open for editing after creation option is enabled and click OK. The Workspace Footprint will be created and the temporary PCB footprint editor will open, presenting a .PcbLib document as the active document. This document will be named according to the Item-Revision, in the format: <Item><Revision>.PcbLib (e.g., PCC-001-0001-1.PcbLib). Use the document to define the footprint as described below.

    Example of editing the initial revision of a Workspace Footprint – the temporary PCB footprint editor provides the document with which to define your footprint.
    Example of editing the initial revision of a Workspace Footprint – the temporary PCB footprint editor provides the document with which to define your footprint.

  3. When the footprint is defined as required, save it to the Workspace using the Save to Server control to the right of the footprint's entry within the Projects panel. The Edit Revision dialog will appear, in which you can change Name, Description, and add release notes as required. The document and editor will close after saving.

A saved Workspace Footprint can be used when defining a component using the Component Editor in its Single Component Editing mode or Batch Component Editing mode.

Workspace Footprints can be browsed using the Components panel. Enable visibility of models by clicking the  button at the top of the panel and selecting Models, then select the Footprints category.

To edit a Workspace Footprint, right-click its entry in the Components panel and select the Edit command. Once again, the temporary editor will open, with the footprint opened for editing. Make changes as required, then save the document into the next revision of the Workspace Footprint.

You can also update the Workspace Footprint being used by a Workspace Component directly on-the-fly, as part of editing that Workspace Component in the Component Editor in its Single Component Editing mode or Batch Component Editing mode.
  • From a designer's perspective, a Workspace Component gathers together all information needed to represent that component across all design domains, within a single entity. It could therefore be thought of as a container in this respect – a 'bucket' into which all domain models and parametric information is stored. In terms of its representation in the various domains, a Workspace Component doesn't contain the Workspace domain models themselves, but rather links to these models. These links are specified when defining the component.
  • PCB footprints can also be created in the Workspace as part of importing existing, older generation (SchLib, PcbLib, IntLib, DbLib, SVNDbLib) libraries of components. The interface to this process – the Library Importer – presents an intuitive flow that takes initial selected libraries, and imports them to your Workspace. Learn more about the Library Importer.
  • A new Workspace Footprint can also be created when defining a Workspace Component in the Component Editor in its Single Component Editing mode.
  • A footprint can also be created as part of a file-based PCB footprint library.

Defining a PCB Footprint

Footprints are always built on the top side, regardless of which final side of the board they are placed, using the same set of tools and design objects available in the PCB editor. Layer-specific attributes, such as surface mount pads and solder mask definitions, are automatically transferred to appropriate bottom-side layers when you flip the footprint to the other side of the board during component placement.

Design objects can be placed on any layer, however, the outline is normally created on the Top Overlay (silkscreen) layer and the pads on the multi-layer (for thru-hole component pins) or the top signal layer (for surface mount component pins). When you place the footprint on a PCB, all objects that make up the footprint will be assigned to their defined layers.

The footprints shown on this page are only to illustrate the procedures required; they are not dimensionally accurate. Always check the specifications of a new footprint against the manufacturer's datasheet.

Manually Creating a Footprint

2D and 3D views of a footprint for a joystick component. The 3D image shows the imported STEP model for the component. Note that the pads and component overlay can be seen below the STEP model. 2D and 3D views of a footprint for a joystick component. The 3D image shows the imported STEP model for the component. Note that the pads and component overlay can be seen below the STEP model.

The typical sequence for manually creating a component footprint is:

  1. Prepare the design space: define snap options, configure grids and guides - learn more.
  2. Footprints should be built around the design space reference point at the center of the PCB footprint editor. This reference point is actually the relative origin for the design space and is the point by which the component footprint is picked-up by the cursor in Place and Move operations. Use the J, R shortcut keys to jump directly to the reference point. If you have forgotten to move to the reference point before beginning to build your footprint, you can bring the reference pad to your footprint using the Edit » Set Reference sub-menu commands:
    • Pin 1 - set the component reference point to be pin 1 of the component footprint.
    • Center - set the component reference point to be the center of the component footprint.
    • Location - set the component reference point to a user-defined location.

    The chosen point will be set to 0,0 - it becomes the new relative origin and all primitives will have their locations updated relative to this point.

  3. Place the pads (Place » Pad) according to the component requirements. After running the Place Pad command but prior to placing the first pad, press the Tab key to open the Properties panel to define all the pad properties, including the pad Designator, Size and Shape, Layer, and Hole Size (for a thru-hole pad). The Designator automatically increments for subsequent pad placements. For a surface mount pad, set the Layer to Top Layer. For a thru-hole pad, set the Layer to Multi-Layer.

    Some footprints require pads that have an irregular shape. This can be done using pad objects of Custom Shape. To learn more, refer to the Customizing a Pad Stack page.
    • One of the most important procedures in creating a new component footprint is placing the pads that will be used to solder the component to the PCB. These must be placed in exactly the right positions to correspond to the pins on the physical device.
    • Some care should also be exercised when designating pads since it is this property that Altium Designer uses when mapping from pin numbers on the schematic symbol.
  4. To ensure accurate placement of the pads, consider setting up a grid specifically for the task. Use the Ctrl+G shortcut keys to open the Cartesian Grid Editor dialog and the Q key to toggle the grid from Imperial to Metric.
  5. To accurately place a pad while moving it with the mouse, use the keyboard arrow keys to move the cursor in current grid increments. Additionally, holding Shift will move in steps of 10 times the grid. The current X, Y location is displayed on the Status bar and also in the Heads Up display. The Heads Up Display contains both the location and the delta from the last click location to the current cursor location. Use the Shift+H shortcut to toggle the Heads Up display on and off. Alternatively, double-click to edit a placed pad and enter the required X and Y locations in the Properties panel.
  6. To check a distance between two points in the design space, use the Reports » Measure Distance (shortcut Ctrl+M). Follow the prompts on the Status bar.
  7. Pad-specific attributes, such as solder mask and paste mask, are automatically calculated based on the pad dimensions and applicable mask design rules. While mask settings can be defined manually for each pad, doing so makes it difficult to modify these settings later during the board design process. Typically this is done only when it is not possible to target the pads by design rules. Note that rules are defined in the PCB editor during board design.
  8. Use tracks, arcs and other primitive objects to define the component outline that appears on the PCB silkscreen on the Top Overlay layer. If the component is flipped to the bottom of the board during placement, the overlay is automatically transferred to the Bottom Overlay layer.
  9. Place tracks and other primitive objects on a mechanical layer to define extra mechanical detail, such as a placement courtyard. Mechanical layers are general-purpose layers. You should allocate the function of these layers and use them consistently across their footprints.
  10. Place 3D Body objects to define the three-dimensional shape of the physical component to be mounted on the PCB.

    A 3D Body object added to a footprint may make reference to a 3D model uploaded to the connected Workspace.
  11. The Designator and Comment strings are automatically added to the footprint’s Overlay layer during placement into the PCB design space. Additional Designator and Comment strings can be included by placing the .Designator and .Comment special strings on a mechanical layer.

    When placing Designator and Comment strings, a Layer Pair needs to be defined in the PCB editor. This ensures that the strings will be tied to the side of the board on which the component is mounted and must flip to the other side of the board when the component is flipped. For more information, see the Handling Special Layer-specific Requirements section below.
  12. Define the properties of the footprint (e.g., its name and description) on the Footprint tab of the Properties panel in its Library Options mode (active when no object is selected in the design space, can be accessed using the Tools » Footprint Properties command from the main menus). Refer to the section below to learn more about the options and controls available under the panel's Footprint tab.

For a standardized pad/via definition across all footprints, the Pad/Via library (*.PvLib) can be used for Pad/Via placement.

Preparing the Design Space

The default is to display the grids using dots. If you prefer, grids can be displayed using lines. This is configured in the Grid Editor dialog, accessed by clicking the Properties button in the Properties panel as shown in the image below. Alternatively, press the Ctrl+G shortcut to open the dialog.

In the image, the fine grid is displayed as dots, and the coarse grid is displayed as lines.
In the image, the fine grid is displayed as dots, and the coarse grid is displayed as lines.

Properties Panel

When editing a footprint in the PCB footprint editor and when no design object is currently selected in the design space, the Properties panel presents the Library Options.

The following collapsible sections contain information about the options and controls available under the panel's General tab:

The following collapsible sections contain information about the options and controls available under the panel's Footprint tab:

When a design object is selected, the panel will present options specific to that object type. The following table lists the object types available for placement within the library design space – click a link to access the properties page for that object.

3D Body Arc
Arc Keepout Fill
Fill Keepout Pad
Region Region Keepout
Text (String, Text Frame) Track
Track Keepout Via

Creating a Footprint Using the IPC Compliant Footprint Wizard

The IPC Compliant Footprint Wizard generates a PCB footprint that is truly compliant with Revision B of the IPC standard 7351 - Generic Requirements for Surface Mount Design and Land Pattern Standard. Rather than working directly from footprint dimensions (as the Footprint Wizard does), the IPC Compliant Footprint Wizard uses dimensional information from the component itself, and then calculates suitable pad and other footprint properties in accordance with the algorithms released by the IPC.

Instead of requiring you to enter the properties of the pads and tracks that are used to define the footprint, the Wizard takes the actual component dimensions as its inputs. Based on the formulas developed for the IPC-7351 standard, the Wizard then generates the footprint using standard Altium Designer objects, such as pads and tracks.

This dialog is compliant with Revision B of the IPC standard 7351 - Generic Requirements for Surface Mount Design and Land Pattern Standard. IPC-7351B was released in 2010 and supersedes IPC-7351A (which was released in 2007).

Functionality is provided courtesy of the IPC Footprint Generator extension (a Software Extension).

The IPC Footprint Generator extension
The IPC Footprint Generator extension

The IPC Footprint Generator functionality can only be accessed provided the IPC Footprint Generator extension is installed as part of your Altium Designer installation. This extension is installed by default when installing the software, but in case of inadvertent uninstall can be found on the Purchased tab of the Extensions and Updates page (click on the  control at the top right of the design space then choose Extensions and Updates from the menu). If reinstalling, remember to restart Altium Designer once the extension has been successfully downloaded and installed.

  One of the supported packages in the IPC Compliant Footprint Wizard is the DPAK (Transistor Outline).

  • Select Tools » IPC Compliant Footprint Wizard to run the IPC Compliant Footprint Wizard.
  • The wizard can create the following footprint type: BGA, BQFP, CAPAE, CFP, CHIP Array, DFN, CHIP, CQFP, DPAK, LCC, LGA, MELF, MOLDED, PLCC, PQFN, PQFP, PSON, QFN, QFN-2ROW, SODFL, SOIC, SOJ, SON, SOP/TSOP, SOT143/343, SOT223, SOT23, SOT89, SOTFL, and WIRE WOUND.
  • The IPC Compliant Footprint Wizard uses dimensional information from the component itself in accordance with the standards released by the IPC.
  • Paste Masks are split into small fills for packages with a large thermal pad (sized 2.1mm x 1.6mm, or larger).

  • For packages involving gullwing leads, pads are trimmed to prevent them from otherwise extending under the package's body.
  • For small packages having a large central thermal pad, the peripheral pads are trimmed to ensure required clearance between the pads in accordance with the IPC Standard.
  • When pad trimming is applied, a warning is displayed within the dialog.
  • All dimensions are entered into the Wizard in metric (mm) units.
  • When working with a file-based PCB footprint library, use the IPC Compliant Footprints Batch Generator to quickly generate multiple footprints, at multiple density levels.

Some of the IPC Compliant Footprint Wizard features include:

  • Overall packaging dimensions, pin information, heel spacing, solder fillets, and tolerances can be entered and immediately viewed.
  • Mechanical dimensions, such as Courtyard, Assembly, and Component (3D) Body Information, can be entered.
  • The Wizard is re-entrant and allows reviewing and making adjustments easy. Previews of the footprint are shown at every stage.
  • The name and description for the footprint are automatically suggested, but can be changed to suit organizational requirements.
  • In accordance with the IPC standard, the Wizard supports three footprint variants (_L_N_M), each tailored to suit a different board density.
  • The Finish button can be pressed at any stage to generate the currently previewed footprint. If you click Finish before completing the entire Wizard, the footprint will be created using the system defaults for the component type you selected.

Selecting the Component Type

Choose the family of components for which you want to create a footprint on the Select Component Type page.

Click on the component type desired. The preview region on the right-hand side of the Wizard dynamically changes to show the currently selected component and also states the type of packages that are allowed to be generated.

The following table lists the component types and packages that are supported in the Wizard.

Included Packages
BGA Ball Grid Array BGA, CGA
BQFP Bumpered Quad Flat Pack BQFP
CAPAE Electrolytic Aluminum Capacitor CAPAE
CFP Ceramic Dual Flat Pack - Trimmed and formed Gullwing Leads CFP
Chip Array Chip Array Chip Array
DFN Dual Flat No-lead DFN
CHIP Chip Components, 2-Pins Capacitor, Inductor, Resistor
CQFP Ceramic Quad Flat Pack - Trimmed and formed Gullwing Leads CQFP
DPAK Transistor Outline DPAK
LCC Leadless Chip Carrier LCC
LGA Land Grid Array LGA
MELF MELF Components, 2-Pins Diode, Resistor
MOLDED Molded Components, 2-Pins Capacitor, Inductor, Diode
PLCC Plastic Leaded Chip Carrier, Square - J Leads PLCC
PQFN Pullback Quad Flat No-Lead PQFN
PQFP Plastic Quad Flat Pack PQFP, PQFP Exposed Pad
PSON Pullback Small Outline No-Lead PSON
QFN Quad Flat No-Lead QFN, LLP
QFN-2ROW Quad Flat No-Lead, 2 Rows, Square Double Row QFN
SODFL Small Outline Diode, Flat Lead SODFL
SOIC Small Outline Integrated Package, 1.27mm Pitch - Gullwing Leads SOIC, SOIC Exposed Pad
SOJ Small Outline Package - J Leads SOJ
SON Small Outline Non-Lead SON, SON Exposed Pad
SOP, TSOP Small Outline Package - Gullwing Leads SOP, TSOP, TSSOP
SOT143/343 Small Outline Transistor SOT143, SOT343
SOT223 Small Outline Transistor SOT223
SOT23 Small Outline Transistor 3-Leads, 5-Leads, 6-Leads
SOT89 Small Outline Transistor SOT89
SOTFL Small Outline Transistor, Flat Lead 3-Leads, 5-Leads, 6-Leads
WIRE WOUND Precision Wire Wound Inductor, 2-Pins Inductor

Preview Region

On the following pages for each component type, the Preview region dynamically updates to show new location, size, etc., for several settings. In the Preview region, you can click  or  to toggle between 2D and 3D preview images.

3D STEP Models

Previewing 3D STEP Models

If desired, you can see a preview of the 3D STEP model before generating the model. Click Generate STEP Model Preview on any page in the Wizard after selecting the component type to see a preview of the 3D STEP model in the Preview region.

The default setting for the files that are created when 3D STEP models are generated is Embedded STEP files. If these default settings are correct for your needs, you can click Finish to exit the IPC® Compliant Footprint Wizard and generate the 3D STEP model.

The subsequent pages of the Wizard change depending upon the component type you selected. Find your component type in the following list then click on the link to access the information regarding that component type. 

Choosing the Footprint Name and Description

The Footprint Description page is used to name and describe your new footprint. Altium Designer uses the information you input in the Wizard to suggest a name and description. Enable Use suggested values to use the Name and Description the system has entered. Enter any desired changes directly in the textboxes.

Selecting the Footprint Destination

Use the Footprint Destination page to select the location for the newly-created footprint to be stored. 

Select Existing PcbLib File if you want the footprint stored in an existing PCB Library file. You can enter the file directly in the textbox or use the  to open a dialog to search for the desired file.

Select New PcbLib File if you want to store the footprint in a new PCB Library file. Enter the name of the new PCB Library file in the textbox. The system will append the new library file name with the extension .PcbLib

Select Current PcbLib File to store the footprint in the displayed PCB Library file.

Enable Produce 3D/STEP model to generate a 3D STEP model.

If you have a valid 'MCAD Co-Designer - SOLIDWORKS(R)' license, you can choose to save the model as file type Parasolid. Click the drop-down to the right of Format then select Parasolid. The file shown in the External File text box is now a *.x_t file.  This is the name and location of the file that will be saved. 

Select either Embedded (default) or External File. Select External File to save your 3D STEP model as an external file. The default file type is STEP and the file name appears in the External File text box with *.step as the file extension. If desired, click  to browse and select the folder in which to save your generated 3D STEP model.

Closing the Wizard

Click Finish to close the Wizard.

Creating a Footprint Using the Footprint Wizard

The PCB footprint editor includes a Footprint Wizard. This Wizard allows you to select from various package types and fill in appropriate information and it will then build the component footprint for you. Note that in the Footprint Wizard you enter the sizes required for the pads and component overlay.

To launch the Footprint Wizard, select Tools » Footprint Wizard from the main menus or right-click in the design space and choose the Tools » Footprint Wizard command from the context menu. Follow the Footprint Wizard's intuitive pages to set up the particular component footprint as required.

Wizard Navigation

  • Click Cancel to close the Footprint Wizard.
  • Click Back to navigate to the previous screen.
  • Click Next to navigate to the next screen.
  • Click Finish to close the Footprint Wizard. This option is available only on the final page of the Wizard.

Selecting Component Patterns

Use the Component patterns page to specify the pattern of the component you want to create. 

Select the desired pattern from the list then use the drop-down to select the unit for the component (Imperial (mil) or Metric (mm)).

The subsequent pages of the Wizard change depending upon the component pattern selected. Find the desired component pattern in the following list then click on the link to access the information regarding that component pattern.

Setting the Component Name

Enter a name for the component in the textbox. 

Completing and Closing the Wizard

Click Finish to close the Wizard.

Solder and Paste Mask Expansions

To check that solder and/or paste masks have been correctly defined in the PCB footprint editor, open the View Configuration panel and enable the show option ( ) option for each mask layer.

The ring that appears around the edge of each pad in the color of the Top Solder Mask layer represents the edge of the solder mask shape protruding by the expansion amount from under the multi-layer pad because multi-layer is at the top of the layer drawing order; it is drawn on top. The Layer Drawing Order is set on the PCB Editor - Display page of the Preferences dialog).

The image below shows a PCB footprint with a purple (color of the Top Solder Mask layer) border that appears around the edge of each pad.

To quickly walk through layers, use the Single Layer Mode (Shift+S) in combination with Ctrl+Shift+Wheel roll.

By default, the shape that is created on the mask layers is the pad shape, expanded or contracted by the amount specified by the Solder Mask Expansion and Paste Mask Expansion design rules set in the PCB on which the footprint is placed. In some cases, you might need to override the expansion design rules and specify a mask expansion as a pad attribute, select from a standard set of predefined mask shapes, or create your own custom shape. In these situations, you can configure paste/solder masks for a selected pad in its Properties panel - learn more. Alternatively, you can place suitable primitives (Regions, Tracks, etc.) on the required mask layer.

Parameter Support

Parameters applied to objects in Altium Designer provide a powerful and flexible means of adding additional information to a PCB design. Applied as properties of the parent object, parameters can be applied at a range of levels, including projects, documents, templates, and individual objects within a design document.

See the Parameter object for more information.

Parameters that become available in the PCB space can be used to filter Queries, Design Rules, Scripts, and Variants, and can be applied in PCB component libraries for invoking custom strings in placed Footprints.

Parameters via an Engineering Change Order

The PCB parameter capabilities are based on functionality included in the ECO mechanism and PCB document, which allow user-defined component parameters to be transferred to and retained in the PCB space. This is a one-way transfer and the passed parameters are read-only in the PCB domain.

The parameter transfer is done by creating an ECO from the schematic to PCB with the Design » Update PCB Document menu command.

When the ECO is executed (by using the Execute Changes button), any new user-defined schematic component parameters will be transferred to the corresponding footprint reference in the PCB design. 

The detection and migration of parameters to the PCB is determined by the project's options settings (Project » Project Options). In the Project Options dialog, set the difference detection and modification behavior in the Differences Associated with Parameters section of the Comparator tab and the Modifications Associated with Parameters section of the ECO Generation tab.

To view the transferred parameters in the PCB editor, double-click a component to open the Properties panel then choose the Parameters tab. The tab will list the current user parameters that have been assigned to the selected component footprint. Parameters for a selected component footprint also are available in the Components panel.

Information Reference Links

The PCB domain automatically accepts the predefined ComponentLink parameters from the schematic. These are defined as parameter pairs (Description and link URL) that normally establish data reference links to specific files or internet locations – typically a manufacturer web site or datasheet URL.

See Defining Clickable Links to Reference Information in a schematic library and Accessing Clickable Links to Reference Information in a PCB document for information on Reference Link parameters.

In both the schematic and PCB design space, the links are accessed from the right-click context menu when hovering over a component (under the References sub-menu options). The specialized parameters are added in the Properties panel, and when transferred to the PCB space, they appear as a component footprint parameter. 

Parameters in Source Footprints

Parameters passed to the PCB can be used for providing additional board production or functional information via component footprints. By adding special parameter strings to footprints at the source library level, the custom strings will be interpreted on the target mechanical layer or overlay.

A special string representing a user-defined parameter can be added to the source component footprint using the special strings button and drop-down ( ) in the Properties panel.

In the below library footprint, the special string .Designator has been placed on the Mechanical 2 layer.

A special string representing a user parameter can be added to the component footprint.

A special string representing a user parameter can be added to the component footprint.

When that custom parameter has also been applied to schematic components and the parameter data has been transferred to the PCB, the interpreted footprint strings will appear on both the board view and generated output files. In this case the special parameter string contains a custom component part identifier to aid assembly.

The application of the user parameters to component footprints as special strings can serve a range of other custom PCB requirements, including function labels for switches and connectors, where a 'function' parameter string might be placed on the Top Overlay in footprints for those component types.

To see the interpreted value of special strings on the board layout, enable Special Strings option under the Additional Options region of the View Options tab in the View Configuration panel. Special strings are always converted in generated output files.
In the schematic editor, if desired, enable the Display Names of Special Strings that have No Value Defined option on the Schematic – Graphical Editing page of the Preferences dialog.

Parameter Queries

Parameter strings in the PCB domain are also accessible through the Altium Designer query language, and therefore, are available for object filtering functions, including the Find Similar Objects feature.

To perform a similar objects selection, right-click on a component then select Find Similar Objects from the context menu to open the Find Similar Objects dialog.

The Find Similar Objects dialog includes a Parameters section where the filtering options can be selected as required.

The PCB Filter panel can apply parameter-specific query words as filter criteria, and can be used for creating Design Rules based on PCB parameters.

Several query words are available for working with PCB footprint parameters, including specific function words for converting string values to numbers (such as StrToNumber). The string Value conversions are unit-aware (V, mA, mV, kOhm etc.,) and allow the query result to be determined by the numerical processing of a parameter value string.

The supported Unit Types that can be nominated in the queries are:

  • % – Percent
  • A – Current
  • C – Temperature
  • dB – Decibels
  • F – Capacitance
  • G – Conductance
  • H – Inductance
  • Hz – Frequency
  • Kg – Mass
  • m – Length
  • Ohm – Resistance
  • Q – Charge
  • s – Time
  • V – Voltage
  • W – Power
  • Z – Impedance

Several Parameter query words are available for working with PCB component footprint parameters.

Several Parameter query words are available for working with PCB component footprint parameters.

The example shown in the Query Helper dialog above processes the Voltage Rating parameter for each component (using the string-to-number conversion – StrToNumber(Unit Value, Unit Type))  to determine if its value is greater than 50V. When applied in the PCB Filter panel, the example board layout exposes a single high-voltage component, C1 (which has a Voltage Rating value of 3kV).

Scientific E notation is also supported, so, for example, a query to filter capacitor values over 1nF would be similar to:
StrToNumber(ParameterValue('CapacitanceValue'), F) > 1e-9
Alternatively, the number conversion function could be used for both the returned ParameterValue and the comparison value:
StrToNumber(ParameterValue('CapacitanceValue'), F) > StrToNumber('1nF', F)

Rules and Scripts

PCB parameter queries can also be applied to Altium Designer Scripts and Design Rules. The latter might perform layout validation checks, such as detecting footprint parameters in order to assess component placement or layer assignment. Note that the functions listed in the Query Helper dialog above are available to the Scripting language.

The below example shows the capacitor voltage rating query (see the filter query above) applied to a component placement rule, which, when run, checks for specific clearance values for components detected as high voltage (>50V) devices.

Design rules defined by specific footprint parameters, as transferred from the schematic space, can be used for detecting custom layout conditions.

Design rules defined by specific footprint parameters, as transferred from the schematic space, can be used for detecting custom layout conditions.

Similarly, custom PCB parameters can be used to check component layer compatibility, for example, where a component does not support wave soldering and therefore placement of the Bottom Layer. Here, an object matching query that processes a custom ‘WaveSoldering’ parameter (Yes/No) might be applied to the Permitted Layers Rule.

The (batch) Rule will subsequently check the value of that component parameter and create a violation if a component is not compatible with placement on the Bottom Layer.


Parameters transferred to the PCB that are included in variations of the design (Design Variants) are processed with Variant selection.

In practice, a varied component parameter in the PCB space will be dynamically detected by a query string, or, for example, displayed on a board layer through a special string. 

User-defined Footprint Parameters

User-defined parameters for footprints are supported in Altium Designer. The Parameters region on the Footprint tab of the Properties panel in its Library Options mode can be used to view and edit footprint parameters when no object is selected in the PCB footprint editor design space.

When the component is placed on the PCB, you can see these parameters in the Properties panel in the Component mode on the Parameters tab.

  • Footprint parameters of components placed on a PCB will be propagated to footprints in libraries generated by the Make PCB Library or Make Integrated Library command of the PCB editor's main menu.
  • Footprint parameters are supported by Altium Designer’s Comparison engine and for generated Pick and Place and ODB++ output.
Altium MCAD CoDesigner supports the placement of native MCAD components in the MCAD according to the configured linking. In some cases, several footprints with different models are linked to one component (e.g., a LED that can be mounted on a PCB in two ways: vertically, with straight legs, or horizontally, with bent legs). Using the footprint parameters, you can now refer to the different MCAD models from those different footprints. Learn more about Linking Native ECAD and MCAD Design Components.

Designator and Comment Strings

Default Designator and Comment Strings

When a footprint is placed on a board, it is given a Designator and Comment based on information extracted from the schematic view of the design. Placeholders for the Designator and Comment strings do not need to be manually defined since they are added automatically when the footprint is placed on a board. The locations of these strings are determined by the Designator and Comment string Autoposition option in the Properties panel in Parameter mode when the designator or comment string is selected in the design space. The default position and size of Designator and Comment strings are configured in the respective Primitive on the PCB Editor - Defaults page of the Preferences dialog.

Additional Designator and Comment Strings

There may be situations when you want additional copies of the designator or comment strings. As an example, your assembly house wants a detailed assembly drawing with the designator shown within each component outline, while your company requires the designator to be located just above the component on the component overlay on the final PCB. This requirement for an additional designator can be achieved by including the .Designator special string in the footprint. A .Comment special string also is available for stipulating the location of the comment string on alternate layers or locations.

To cater to the assembly house's requirements, the .Designator string would be placed on a mechanical layer in the library editor and printouts that included this layer could then be generated as part of the design assembly instructions.

Handling Special Layer-specific Requirements

There are a number of special requirements a PCB component can have, such as needing a glue dot or a peel-able solder mask definition. Many of these special requirements will be tied to the side of the board on which the component is mounted and must flip to the other side of the board when the component is flipped.

Rather than including a large number of special-purpose layers that may rarely be used, Altium Designer's PCB editor supports this requirement through a feature called layer pairs. A layer pair is two mechanical layers that have been defined as a pair. Whenever a component is flipped from one side of the board to the other, any objects on a paired mechanical layer are flipped to the other mechanical layer in that pair. Using this approach, you select a suitable mechanical layer to include the glue dot (or other special requirements) and define its shape using the available objects. When you place that footprint onto a board, you must set up the layer pairing. This instructs the software on which layer it must transfer objects to when this component is flipped to the other side of the board. You cannot define layer pairs in the PCB footprint editor; this is done in the PCB editor.

Layer Pairing needs to be defined before the component gets flipped. If the pairing is defined after the component has moved to the bottom side, the mechanical contents will flip but stay on their original layer. If you forget to create layer pairs before flipping, you can update from the library to refresh the instance of the component placed on the board.

The Names of Mechanical Layers can be edited directly from the View Configurations panel by right-clicking then selecting Edit Layer.

A common approach to managing mechanical layer usage is to assign a dedicated layer number for each required mechanical layer function. This approach requires all designers to adhere to the same layer assignment and numbering scheme. It can also create difficulties when components are obtained from other sources that do not follow the same assignment and numbering scheme. If a different scheme has been used, the design objects must be moved from their current mechanical layer to the mechanical layer assigned for that function.

This issue is resolved with the introduction of the Layer Type property. When a component is placed from a library into the PCB editor, or copied from one library to another, or created by the IPC Footprint Wizard, existing Layer Type assignments are automatically matched, regardless of the mechanical layer number(s) assigned to those Layer Types. The objects are relocated on the correct layer(s) according to their Layer Type. If the software is unable to match by Layer Type, it will fall back to matching by Layer Number.

For both individual mechanical layers and Component Layer Pairs, you can select a Layer Type from a pre-defined list of types. You may access the dialogs shown below by right-clicking on an individual layer, then selecting the Edit Layer or Add Component Layer command from the menu.

For detailed information about component-related mechanical layer types, refer to the Working with Mechanical Layers page.

Adding Height to a PCB Footprint

At the simplest level of 3D representation, height information can be added to a PCB footprint. To do this, open the Properties panel in its Library Options mode (active when no object is selected in the design space) and enter the recommended height for the component in the Height field on the Footprint tab of the panel.

Height design rules can be defined during board design (click Design » Rules in the PCB Editor), typically testing for maximum component height in a class of components or within a room definition.

A better option for defining height information would be to attach 3D Bodies to the PCB footprint.

Managing Components With Routing Primitives

When a design is transferred, the footprint specified in each component is extracted from the available libraries and placed on the board. Then each pad in the footprint has its net property set to the name of the net connected to that component pin in the schematic. All objects touching a pad connect to the same net as the pad.

The PCB editor includes a comprehensive net management tool. To launch it select Design » Netlist » Configure Physical Nets from the main menus to open the Configure Physical Nets dialog. Click the Menu button for a menu of options. Click the New Net Name header drop-down to select the net to assign to the unassigned primitives.

Footprints With Multiple Pads Connected to the Same Pin

The footprint shown below, a SOT223 transistor, has multiple pads that are connected to the same logical schematic component pin - Pin 2. To make this connection, two pads have been added with the same designator - '2'. When the Design » Update PCB command is used in the Schematic Editor to transfer design information to the PCB, the resulting synchronization will show the connection lines going to both pads in the PCB editor, i.e. they are on the same net. Both of these can be routed.

SOT223 footprint showing two pads with a designator of 2.
SOT223 footprint showing two pads with a designator of 2.

Silkscreen Preparation

To assist in resolving common Design for Manufacture (DFM) issues faced by having silkscreen overlapping exposed copper and holes, the PCB footprint editor includes a dedicated feature for preparing the silkscreen for your footprints. These issues can be effectively addressed by:

  • automated clipping of silkscreen lines and arcs;
  • automated clipping or movement of fills and regions;
  • automated movement of silkscreen text strings.
The silkscreen preparation tool can also be accessed when designing a PCB: learn more.

To access the silkscreen preparation tool in the PCB footprint editor, use the Tools » Silkscreen Preparation command from the main menus. The Silkscreen Preparation dialog will open.

Use the dialog to configure the settings of the silkscreen object clipping/movement. The available options are:

  • Clip to Exposed Copper – enable to automatically clip objects to exposed copper.
  • Clip to Solder Mask Openings – enable to automatically clip objects to solder mask openings.
  • Silkscreen Clearance – define the minimum acceptable value between silkscreen objects and exposed copper / solder mask openings and holes.
  • Min Remaining Length – if the line/arc length is less than the defined value after clipping, the objects will be removed from the footprint. Note that this length is the vertex-to-vertex length, not the edge-to-edge length (show image).
  • Move Text – enable to move silkscreen text strings away from exposed copper / solder mask openings and holes if the distance between them is less than the Silkscreen Clearance. The movement is limited by the Max Distance value.
  • Fill & Region – select an action to be performed for fills and regions when the distance between them and exposed copper / solder mask openings and holes is less than the Silkscreen Clearance:
    • None – fills and regions remain untouched.
    • Clip – fills and regions will be clipped to maintain the Silkscreen Clearance. Fills are converted to regions if applicable.
    • Move – fills and regions will be moved away from exposed copper / solder mask openings and holes. The movement is limited by the Max Distance value.
  • Max Distance – define a maximum distance to which text strings, component designators, fills and regions can be moved to maintain the Silkscreen Clearance.

Click OK to perform clipping and/or movement of silkscreen objects according to the settings in the dialog.

If an action cannot be performed for an object (e.g., a text string cannot be moved due to the limitation of Max Distance), a message for this object will appear in the Messages panel.

Below is shown an example of the silkscreen preparation tool performance.


Generating a Component Report

To generate a report for the active PCB footprint, choose the Reports » Component command from the main menus. After launching the command, the report will be generated (<PCBLibraryDocumentName>.CMP) in the same folder as the source PCB library document and will automatically be opened as the active document in the main design window. The report lists information including footprint dimensions and a breakdown of the primitive objects that constitute the footprint and the layers on which they reside.

The report will be added to the Projects panel as a free document under the Documentation\Text Documents sub-folder.

Working with Jumper Components

Jumpers, also referred to as wire links, allow you to replace routing with a Jumper component, which is often an essential ingredient to successfully designing a single-sided board.

Early printed circuit boards were all single sided. To successfully implement all of the connections, jumpers or wire links were often used to create another layer of connectivity, which could pass across the printed routing. The image below shows an example of Jumpers being used to implement the routing on one side of the board.

Note the representation of a Jumper, with a curved connection line between the two pads. In the image, the jumper connection lines are shown in different colors because they inherit the color assigned to the net.

What Defines a Jumper?

To act as a jumper, you need:

  • The component Type set to Jumper.
  • The Jumper value set to the same, non-zero value for pads in the Jumper component.

How Jumpers are Used

After placing a Jumper in the design space you will need to set the Net attribute of one of the pads manually in the Properties panel since there is no automatic net inheritance. Note that if the component is defined as a Jumper, then the other pad will automatically inherit the same Net name.

Controlling the Display of Jumpers

The View menu includes a Jumpers sub-menu that allows control over the display of Jumper components.

There are also Jumper sub-menus in the Netlist popup menu (N shortcut).

Use the available commands to:

  • Show or hide all jumpers for the design.
  • Show or hide the jumper connection lines with respect to components associated with a single net.

    If you do not know the location of a pad on the net, or one of its connection lines, click in free space and a dialog will pop up, prompting for the net name. If you are unsure of the net name, type ? and click OK to launch the Nets Loaded dialog, which lists all loaded nets for the design. The connection lines for the net you choose in the dialog will be hidden when you click OK.

  • Show or hide the jumper connection lines for a particular component.

    If you do not know the location of a component, click in free space and a dialog will pop up, prompting for the component's designator. If you are unsure of the designator, type ? and click OK to launch the Components Placed dialog, which lists all components in the design. The connection lines for all nets associated to the component you choose in the dialog will be hidden when you click OK.

The query keyword IsJumperComponent is available for filtering and rule definition.

Jumpers and the Bill of Materials

Jumpers are typically pieces of tinned copper wire that are bent to the correct length, meaning they need to be in the BOM. To support this, Jumpers also can be included on the schematic so that they are included in the Bill of Materials. The Synchronizer and the Report engine have the following behavior for synchronizing Jumpers:

  • The component itself is synchronized.
  • Net properties of Jumper pins are not synchronized.
  • The Jumper is included in the BOM.

Suggested Workflow for Working with Jumpers

The following description is one approach to working with Jumper components. This workflow starts at the schematic, but you can also start by placing the Jumper footprints directly onto the PCB. The main reason for starting on the schematic is that when the design is transferred to the PCB workspace, the footprints will have the correct component Type of Jumper. If you place them directly from the PCB library into the PCB workspace, the component Type will default to Standard, so you will need to manually set it.

Create the Jumper Footprints

Create a footprint for each length jumper that will be used. Typically jumpers are designed in pre-defined lengths, for example, in increments of 0.1 inch (100 mils).

As mentioned above, there are two conditions that make a Jumper a Jumper:

  • Both pads in the Jumper must have their Jumper value set to the same, non-zero value in the Properties panel. Note that it does not matter if the pads in all Jumper footprints used on a board design have the same Jumper value.
  • The Jumper Component must have its Type set to Jumper in the Properties panel. Note that this can only be set once the footprint has been placed into the PCB workspace; it cannot be set in the PCB Library editor.

The image below shows a typical Jumper in the PCB Library editor. Both pads have the Jumper value of 1.

Create the Schematic Jumper Component

On the schematic side, you can either:

  • Create a single Jumper component, then add to it all of the different length Jumper footprints that you need.
  • Create an individual Jumper component for each different length Jumper footprint that will be used.

Once the symbol has been created:

  1. Set the default Designator.
  2. Set the Component Type to Jumper.
  3. Add the various Jumper footprints to the Models list.
  4. Define the other component properties you need, such as the Description and any required component Parameters on the Parameters tab.

Placing Jumpers onto the Schematic

Once the Jumper has been designed, you can place a number of them onto the schematic. At this stage, you probably do not know how many you will need, however, extras can easily be deleted. Keep in mind they are on the schematic to ensure they go into the BOM; they do not need to be wired into the circuit at each location that they end up being used. For that reason, it makes sense to place them all on the same schematic sheet, perhaps with other BOM-only hardware, such as screws.

When a Design » Update PCB Document command is performed, all of the jumpers will be placed into the PCB workspace using the default footprint to the right of the board shape.  

Position and Routing the Jumpers on the PCB

The image below shows the PCB, almost completely routed. Note the remaining connection lines showing where the routes are not complete. There are also a number of un-placed Jumper components to the right of the board.

The routing for each of these connections cannot be completed because there is no route path available on this single-sided design. To complete them, the Jumper components will be used.

To complete a connection with a Jumper:

  1. Drag a jumper component into position on the board. If it is not long enough, either press Tab while moving the Jumper or double-click once it is placed to open the Component mode of the Properties panel.
  2. In the Footprint region of the Properties panel, enter the Footprint Name, or click the  to open the Browse Libraries dialog to select a footprint.
  3. To make it easier to include the Jumper in the BOM, enter a suitable identifying string in the Comment field. In the image below, the footprint name has been copied and pasted into the Comment field since it describes how long the jumper is.

  4. Position the Jumper in the required location.
  5. Double-click to edit one of the pads then select the required net name from the Net drop-down list in the Properties region of the Properties panel. The other pad in the Jumper will automatically be assigned the same net name.

  6. Once all Jumpers have been placed, delete any unused Jumpers from the board.
  7. Run the Design » Update Schematics command to push the footprint and comment changes back to the schematic.
  8. The last step is to remove any unused Jumper components from the schematic. These can be identified by switching to one of the schematic sheets and running the Design » Update PCB Document command. The Engineering Change Order dialog will open and list any extra components on the schematic; note their designators then close the ECO dialog and delete those excess Jumpers from the schematic.
If you find an issue, select the text/image and pressCtrl + Enterto send us your feedback.

The features available depend on your Altium product access level. Compare features included in the various levels of Altium Designer Software Subscription and functionality delivered through applications provided by the Altium 365 platform.

If you don’t see a discussed feature in your software, contact Altium Sales to find out more.