Component

Parent page: PCB Dialogs

The Component Dialog.

Summary

The Component dialog is used to edit the properties of the selected component. The Component footprint defines the space and connection points needed to mount the physical component on the printed circuit board.

Access

The dialog can be accessed during Component placement:

  • By pressing the Tab key.

After placement, the dialog can be accessed in the following ways:

  • Double-clicking on a Component footprint.
  • Placing the cursor over a Component, right-clicking and selecting the Properties command from the context menu.

Options/Controls

Component Properties

  • Layer - Sets the layer that the component is placed on. Components can be assigned to the Top layer or Bottom layer, click to select a different layer. Changing the layer status swaps all of the component primitives to each layer's respective opposite layer. For example, moving a Top layer component to the Bottom layer means: single layer pages are swapped from the Top to the Bottom layer; primitives on the Top Overlay are reassigned to the Bottom Overlay; and primitives on a paired mechanical layer are swapped to the other mechanical layer in that pair. The orientation of the component will be flipped along the X-axis and the component overlay text will read from the bottom. To flip a component during placement, press the L key while the component is floating on the cursor.
  • Rotation - The component's angle of rotation (in degrees), measured anti-clockwise from zero (the 3 o'clock horizontal). Edit to change the rotation of the component. Minimum angular resolution is 0.001°.
  • X-Location - The current X (horizontal) coordinate of the reference point of the component, relative to the current workspace origin. Edit to change the X position of the component. The value can be entered in either metric or imperial, include the units when entering a value whose units are not the current default. The current units used in the dialog can be toggled by pressing the Ctrl+Q shortcut. The reference point for a component footprint is set in the Library Editor.
  • Y-Location - The current Y (vertical) coordinate of the reference point of the component, relative to the current origin. Edit to change the Y position of the component. The value can be entered in either metric or imperial, include the units when entering a value whose units are not the current default. The current units used in the dialog can be toggled by pressing the Ctrl+Q shortcut. The reference point for a component footprint is set in the Library Editor.
  • Type - Select one of the following component types for the component footprint here. The available types are:
    • Standard - These components possess standard electrical properties, are always synchronized between the schematic and PCB (the footprint, pins/pads and net assignments must all match), and are included in the BOM. An example is a standard electrical component, such as a resistor.
    • Mechanical - These components do not have electrical properties, are not synchronized (you must manually place them in both editors), and are included in the BOM. An example is a heatsink.
    • Graphical - These components do not have electrical properties, are not synchronized (you must manually place them in both editors), and are not included in the BOM. An example is a company logo.
    • Net Tie (in BOM) - These components are used to short two or more different nets together, they are always synchronized between the schematic and PCB (the footprint, pins/pads and net assignments must all match), and are included in the BOM. They differ from a Standard component in that connectivity created by copper within the footprint is not checked - it is this copper that allows the nets to be shorted. Note: enable the Verify Shorting Copper option in the Design Rule Check dialog to verify that there is no unconnected copper within the component (Home | Design Rules | Design Rule Check » Design Rule Check).
    • Net Tie - These components are used to short two or more different nets together, they are always synchronized between the schematic and PCB (the footprint, pins/pads and net assignments must all match), and are not included in the BOM. They differ from a Standard component in that connectivity created by copper within the footprint is not checked - it is this copper that allows the nets to be shorted. Note: enable the Verify Shorting Copper option in the Design Rule Check dialog to verify that there is no unconnected copper in the component (Home | Design Rules | Design Rule Check » Design Rule Check).
    • Standard (No BOM) - These components possess standard electrical properties, are always synchronized between the schematic and PCB (the footprint, pins/pads and net assignments must all match), and are not included in the BOM. An example is a testpoint component, that you wish to exclude from the BOM.
    • Jumper - These components are used to include wire links in a PCB design, for example on a single-sided PCB that cannot be fully routed on one layer. For this component type the component footprint and pins are synchronized between the schematic and PCB but the net assignments are not, and the component is included in the BOM. As well as selecting this option at the component level, both of the pads in the component must have their JumperID set to the same non-zero value. Jumper type components do not need to be wired on the schematic, they only need to be included on the schematic if they are required in the BOM. If they are not required in the BOM they can be placed directly in the PCB, where the Component Type is set, the JumperIDs are set, and the Nets manually assigned for the pads. 
  • Height - A height field for the component, this field was used before the introduction of the 3D Body object, which provides a superior method of defining the component height.
  • Lock Primitives - Enable this option to lock all the primitives of the component, so that it can be treated as a single object (default is on). Clear this checkbox to modify the individual primitives that make up the component. After editing, the component primitives should be re-locked. Note: component pad properties can be modified without unlocking the primitives by double-clicking directly on the pad.
  • Lock Strings - Enable this option to lock the designator and comment strings of the component. When this option is enabled the designator and comment cannot be interactively moved or edited (default is off).
  • Locked - Enable this option to lock the component in the PCB editor workspace. A locked component cannot be single-click selected or graphically edited. To interactively select and edit that specific object, double click directly on the locked object and disable the Locked property.
  • Hide Jumpers - When a component is configured as a jumper (has a Type of Jumper, and pads with a non-zero, matching JumperID), a curved line is drawn between the pads to represent the jumper wire. Enable this checkbox to hide the curved jumper line.

Designator / Comment

  • Text - Designator (Comment) of this component, an alphanumeric string of up to 255 characters. Each component must have a unique Designator string.
  • Height - The current height of the Designator (Comment) characters. The character width (not the stroke width) is automatically proportioned to the height. A typical minimum height of 36mil (0.9mm) will allow the string to be legibly photoplotted, check with your fabricator before using a smaller size. The text height can range between 0.01 to 10000mil, the value can be defined in either metric or imperial units (include the units if entering a dimension that is not in the current board units).
  • Width - Stroke width, or thickness, of the Designator (Comment) text. The width can range between 0.001 to 255mil, and the value can be defined in either metric or imperial units (include the units if entering a dimension that is not in the current board units).
  • Layer - Layer that the Designator (Comment) is displayed on, the text can be assigned to any available layer.
  • Rotation - The current text rotation angle in degrees, measured anti-clockwise from the zero-degree point of the first quadrant (the 3 o'clock, horizontal right position). Text rotation can be set independently of the component rotation. Minimum angular resolution is 0.001°.
  • X-Location - X coordinate of the text relative to the current workspace origin, the reference point is the bottom left corner of the string.
  • Y-Location - Y coordinate of the text relative to the current workspace origin, the reference point is the bottom left corner of the string.
  • Autoposition - Automatically locate the text in the selected location, if the component is rotated the text will remain in this position.
  • Hide - Hide the text string.
  • Mirror - Mirror the text string.

Designator / Comment Font

  • True Type -Enable this to use a TrueType font for the Designator (Comment). The fonts available will depend on the TrueType fonts installed on your system. TrueType fonts support bold and/or italic attributes. Note: if you are using a font that is not a standard Windows font and the design is to be moved to another PC, embed the fonts within the PCB document by enabling ???.
  • Stroke - A simple, built-in font family of 3 different styles, included with the software.
  • Font Name - Select the Font style from dropdown list.

Swapping Options

  • Enable Pin Swaps - Check this option to allow this component to support pin swapping
  • Enable Part Swaps - Check this option to allow this component to support part swapping

FPGA

  • Color Overlay - For an FPGA part, select from dropdown list to define color overlay for IO bank/CLK pin/Diff Pair/IO pin.

Axes

Axes can be used as a reference when aligning a 3D Body to another PCB object, such as a component footprint. An axis is essentially a dashed line drawn between the points defined by the Origin and Direction X, Y, Z locations. Note that Origin 0, 0, 0 is located on the base of the object, at the geometric center of the component footprint when looking down at it in 2D display mode.

  • Add - attach a new Axis.
  • Delete - remove the currently selected Axis.
  • Origin X, Y & Z - the co-ordinates of the starting point for the axis, click to edit the values.
  • Direction X, Y & Z - the location in space that defines another point that the axis passes through, click to edit the values.

Schematic Reference Information

Schematic reference information that is transferred from the schematic to the PCB editor when the design is initially transferred. To refresh this data at a later stage, click the Perform Update button in the Component Links dialog.

  • Unique ID - The unique identifier (UID) of the schematic component that this PCB component has been matched with.
  • Designator - The designator of the schematic component that this PCB component has been matched with.
  • Hierachical Path - Shows where in the hierarchical structure of the schematic that this component can be found.
  • Description - Description of the schematic component.
  • SCH Library - Name of the schematic library the schematic component was placed from.
  • Library Ref - Name of the schematic library component that this PCB component has been matched with.
  • Channel Offset - When a design is first transferred from schematic to PCB, each component on each schematic sheet is given a unique channel offset. The offset is then used in a multi-channel design when the Copy Room Format command is executed, identifying the instantiation of the component within each room.

Footprint

Detail information for the selected Footprint.

  • Name - Name of this component footprint.
  • Library - Library that this component footprint was placed from.
  • Description - Description of the footprint, the description is defined in the PCB Library editor.
  • Default 3d model - Legacy field for an older 3D view system.
  • Vault Name - Item ID (name of the Item in the Vault) for this footprint, if it was placed from an Altium Vault.
  • Item Revision - Every Vault Item has a Revision, this is the revision of this Item if it was placed from an Altium Vault.

To toggle the units of measurement used in the open dialog between metric (mm) and imperial (mil), press the Ctrl+Q shortcut. This affects the dialog only and does not change the actual measurement unit currently employed for the board, as determined by the Home | Grids and Units | Metric or Imperial setting chosen on the Ribbon.

You are reporting an issue with the following selected text and/or image within the active document: