Configuring PCB Pad Object Properties in Altium Designer

Parent page: Pad

PCB Editor object properties are definable options that specify the visual style, content and behavior of the placed object. The property settings for each type of object are defined in two different ways:

• Pre-placement settings – most Pad object properties, or those that can logically be pre-defined, are available as editable default settings on the PCB Editor – Defaults page of the Preferences dialog (accessed from the  button at the top-right of the design space). Select the object in the Primitive List to reveal its options on the right.

   

   

   

   

   

  

• Post-placement settings – all Pad object properties are available for editing in the Properties panel and the Pad dialog when a placed Pad is selected in the design space.

   

   

   

   

   

   

Net Information (Properties panel only)

• Net Name – the name of the selected net.
• Net Class – the name of the selected net class.
• Total
  • Length – the total Signal Length. The Signal Length is the accurate calculation of the total node-to-node distance. Placed objects are analyzed to resolve stacked or overlapping objects and wandering paths within pads; and via lengths are included. The Pin Package Length is also included if it has been defined for the pad(s). If the net is not completely routed, the Manhattan (X + Y) length of the connection line is also included. For more information regarding Signal Length and its applications, see the PCB – Nets page.
  • Delay – the delay of the routed segments of the Total Length. Includes the Pad and Via Propagation Delay values, if they have been defined for the pads and vias.

• Selected
  • Length – the total length sum of the selected object(s).
  • Delay – the total delay of the selected object(s). Includes selected Pad and Via Propagation Delay values if they have been defined for the pads and vias.

Properties

• Designator – this field displays the current pad designator. If the pad is part of a component, the designator is usually set to the corresponding component pin number. Free pads can include a designator or the field can be left empty. If the designator begins or ends with a number, the number will auto-increment when placing a series of pads sequentially. Edit the value in this field to change the pad designator.
• Layer – this field displays the layer to which the pad is currently assigned. Pads can be assigned to any available layer. To change the assigned layer, click the field and select a layer from the drop-down list.
• Net – use to choose a net for the pad. All nets for the active board design will be listed in the drop-down list. Select No Net to specify that the pad is not connected to any net. The Net property of a primitive is used by the Design Rule Checker to determine if a PCB object is legally placed. Alternatively, you can click on the Assign Net icon () to choose an object in the design space - the net of that object will be assigned to selected pad(s).
• Electrical Type – this field displays the current electrical status of the pad. This status is only relevant for component pads and sets the transmission line characteristics for these pads. Pads can be designated as a Load, Source or Terminator. The Source and Terminator settings are used when a net requires one of the Daisy chain routing topologies. Click the field to change the electrical type from the drop-down list.
• Propagation Delay – this field lists the propagation delay, which is the amount of time it takes for the head of the signal to travel from the sender to the receiver.
• Pin Package Length – the Pin Package Length is automatically included in the Signal Length calculations that are displayed in the PCB panel. Set the PCB panel to Nets mode to examine (or edit) the value of the Pin/Pkg Length for the pins in the chosen net.
• Jumper – this field provides a jumper connection identification number (range of 1 – 1000) to the pad when you are using a jumper connection on the PCB. A jumper connection uses a wire to physically connect pads on a PCB, and not using tracks or electrical objects on the board. The Jumper value tells the software which pads to treat as 'connected'. A jumper connection can only be created among the pads within a component footprint. The pads used must use the same Jumper value and must also share the same net. A jumper connection is shown as a curved connection line in the PCB Editor. Use the scroll arrows or directly enter the desired jumper connection identification number.
• Template – displays the current template for the pad. Use the drop-down to select another template. If there is an associated Library, that library will be displayed.
• (X/Y)
  • X (first field) – this field shows the current X position of the center of the pad relative to the current origin. Edit the value in the field to change the position of the pad relative to the current origin. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. Default units (metric or imperial) are determined by the Units setting in the Other region of the Properties panel in Board mode (accessed when no objects are selected in the design space), and are used if the unit is not specified.
  • Y (second field) – this field shows the current Y position of the center of the pad relative to the current origin. Edit the value in the field to change the position of the pad relative to the current origin. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. Default units (metric or imperial) are determined by the Units setting in the Other region of the Properties panel in Board mode (accessed when no objects are selected in the design space), and are used if the unit is not specified.
  The icon to the right of this region must be displayed as  (unlocked) in order to access the below fields. Toggle the lock/unlock icon to change its lock status. When locked, no edits can be made to the location
• Rotation – the pad's angle of rotation (in degrees), measured counterclockwise from zero (the 3 o'clock horizontal). this field to change the rotation of the pad. Minimum angular resolution is 0.001°.

Pad Stack Information

• Simple – select to choose a simple layered pad. You can define X and Y sizes and shape attributes that are common for all layers of this pad.
  • Shape – this field shows the current basic pad shape. Basic shapes can be manipulated by changing the X and Y settings to produce asymmetrical pad shapes.
  • (X/Y) – displays the current X (horizontal) and Y (vertical) size of the pad. The values set the size of the pad and can accept values of 1 to 10000mil. The X and Y size can be set independently to define asymmetric pad shapes. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. Default units (metric or imperial) are determined by the Units setting in the Other region of the Properties panel in Board mode (accessed when no objects are selected in the design space) and are used if the unit is not specified.
  • Corner Radius – this displays the corner radius of a pad. Pad radius is represented as a percentage of half of the shortest side of the pad. This option is available only if Rounded Rectangle is selected as Shape.
  • Thermal Relief – check the box to enable thermal relief to reduce heat conductivity. Once checked, click to open the Polygon Connect Style dialog in which you can choose the style of the connection: Relief Connect, Direct Connect, or No Connect.
  • Offset From Hole Center (X/Y) – enter a value to offset the pad landing area from the center of the pad hole.
• Top-Middle-Bottom – select to choose a Top-Middle-Bottom layered pad object. You can define X and Y sizes and shape attributes for top, middle and bottom layers for this pad object.
  • Displayed Layer(s) – click on a displayed layer to configure pads for that layer. The selected layer is highlighted.
  • Shape – this field shows the current basic pad shape. Choices are: Round, Rectangular, Octagonal, and Rounded Rectangle. Basic shapes can be manipulated by changing the X and Y settings to produce asymmetrical pad shapes.
  • (X/Y) – displays the current X (horizontal) and Y (vertical) size of the pad. The values set the size of the pad and can accept values of 1 to 10000mil. The X and Y size can be set independently to define asymmetric pad shapes. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. Default units (metric or imperial) are determined by the Units setting in the Other region of the Properties panel in Board mode (accessed when no objects are selected in the design space) and are used if the unit is not specified.
  • Corner Radius – this displays the corner radius of a pad. Pad radius is represented as a percentage of half of the shortest side of the pad. This option is available only if Rounded Rectangle is selected as Shape.
  • Thermal Relief – check the box to enable thermal relief. Once checked, click  to open the Polygon Connect Style dialog in which you can choose the style of the connection: Relief Connect, Direct Connect, or No Connect.
  • Offset From Hole Center (X/Y) – enter a value to offset the pad landing area from the center of the pad hole.
• Full Stack – select to choose a Full Stack layered pad object. You can define X and Y sizes and shape attributes for all layers for this pad object. 
  • Displayed Layer(s) – click on a displayed layer to configure pads for that layer. The selected layer is highlighted.
  • Shape – this field shows the current basic pad shape. Basic shapes can be manipulated by changing the X and Y settings to produce asymmetrical pad shapes.
  • (X/Y) – displays the current X (horizontal) and Y (vertical) size of the pad. The values set the size of the pad and can accept values of 1 to 10000mil. The X and Y size can be set independently to define asymmetric pad shapes. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. Default units (metric or imperial) are determined by the Units setting in the Other region of the Properties panel in Board mode (accessed when no objects are selected in the design space) and are used if the unit is not specified.
  • Corner Radius – this displays the corner radius of a pad. Pad radius is represented as a percentage of half of the shortest side of the pad. This option is available only if Rounded Rectangle is selected as Shape.
  • Thermal Relief – check the box to enable thermal relief to reduce heat conductivity. Once checked, click to open the Polygon Connect Style dialog in which you can choose the style of the connection: Relief Connect, Direct Connect, or No Connect.
  • Offset From Hole Center (X/Y) – enter a value to offset the pad landing area from the center of the pad hole.
• Round/Rect/Slot – choose the desired hole shape. The image above and options below update accordingly.
  • Round – specifies a round hole shape (the default) for the hole size of a pad. Separate drill files (NC Drill Excellon format 2) are generated for each hole kind, as well as for plated and non-plated holes. There are up to six different drill files for these types.
  • Rect – specifies a rectangle (punched) hole for this pad. Rectangle holes can be plated or unplated. Separate drill file (NC Drill Excellon format 2) are generated for each hole kind, as well as for plated and non-plated holes. There are up to six different drill files for these types.
  • Slot – specifies a round-ended, slotted hole for this pad. Slotted holes can be plated or unplated. Separate drill file (NC Drill Excellon format 2) are generated for each hole kind, as well as for plated and non-plated holes. There are up to six different drill files for these types.
• Hole Size – this field displays the current hole size for the pad. The value specifies the diameter of the hole (as a round, square or slotted shape) in mils or mm to be drilled in the pad during fabrication. For SMD pads or edge connectors, this should be set to zero. The hole size can be set from 0 to 1000mil and can be set larger than the pad to define (copper free) mechanical holes. Edit the value in this field to change the pad hole size. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. Default units (metric or imperial) are determined by the Units setting in the Other region of the Properties panel in Board mode (accessed when no objects are selected in the design space) and are used if the unit is not specified.

• Tolerance – setting hole tolerance attributes can help determine the fits and limits of your board. Specify the minimum (-) and maximum (+) tolerances for the hole. There is no default hole tolerance value in Altium Designer.

  Component datasheets list a tolerance with plus/minus to accommodate variations in aging, wear, temperature, plating, material, machining, and so forth. As holes are drilled, drill bits wear and get smaller, or the drill may vibrate or wiggle slightly in a hole, causing a slightly larger hole. Mounting holes are then plated, and the plating may be thicker or thinner for each batch or position on the board. You also have to account for thermal expansion or shrinkage of the Printed Circuit Board PCB substrate as it is being processed. Therefore, hole tolerance is critical in the design process to accommodate all tolerance, drill wear or wobble, and plating variations.
• Length – displays the length for the hole of the pad. The value specifies the length of the hole in mm or mil, to be NC-routed in the pad during fabrication. The hole size can be set from 0 to 1000mil and can be set larger than the pad to define (copper free) mechanical holes. 
  Edit the value in this field to change the length. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. Default units (metric or imperial) are determined by the Units setting in the Other region of the Properties panel in Board mode (accessed when no objects are selected in the design space) and are used if the unit is not specified. This option is not available if Round is selected.
• Rotation – displays the current hole's counterclockwise rotation in degrees. Edit this field to change the rotation. Minimum angular resolution is 0.001°. This option is not available if Round is selected.
• Plated – this option determines whether or not the pad has a plated hole. A checkmark in this field sets the pad as a plated hole pad. If both plated and non-plated pads exist in a design, the non-plated holes will be set to use different tools from the plated holes in the NC drill files.

Paste Mask Expansion

• Rule – select to have the paste mask expansion for the pad follow the defined value in the applicable Paste Mask Expansion design rule.

• Manual – select to override the applicable design rule and specify the paste mask expansion value for the pad. You can then enter the desired paste mask expansion measurement or disable use of paste mask for the pad. The value can be defined as either an absolute value (mil/mm) or percentage of the pad area. When entering an absolute value, include the units when entering a value whose units are not the current default. Default units (metric or imperial) are determined by the Units setting in the Other region of the Properties panel in Board mode (accessed when no objects are selected in the design space) and are used if the unit is not specified.

  The features for disabling use of paste mask and for defining paste mask expansion as a percentage of the pad area are in Open Beta. If required, they can be turned off  by disabling the PCB.PasteMask.NoPaste and PCB.PasteMask.Percentage options respectively in the Advanced Settings dialog.

Solder Mask Expansion

• Rule – select to have the solder mask expansion for the pad follow the defined value in the applicable Solder Mask Expansion design rule.
  • Top
    • Tented – check if it desired for any solder mask settings in the solder mask expansion design rules to be overridden, which results in no opening in the solder mask on the top layer of this pad and is therefore tented. Disable this option and this pad is affected by a solder mask expansion rule or specific expansion value.
  • Bottom
    • Tented – check if it desired for any solder mask settings in the solder mask expansion design rules to be overridden, which results in no opening in the solder mask on the bottom layer of this pad and is therefore tented. Disable this option and this pad is affected by a solder mask expansion rule or specific expansion value.
• Manual – select to override the applicable design rule and specify the solder mask expansion value for the pad. 
  • Top – enter the top layer solder mask expansion value. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. Default units (metric or imperial) are determined by the Units setting in the Other region of the Properties panel in Board mode (accessed when no objects are selected in the design space) and are used if the unit is not specified. This field is accessible only if Tented is not enabled.
    • Tented – check if it desired for any solder mask settings in the solder mask expansion design rules to be overridden, which results in no opening in the solder mask on the top layer of this pad and is therefore tented. Disable this option and this pad is affected by a solder mask expansion rule or specific expansion value.
  • – you can enter Bottom measurement and Tented options if Bottom layer Solder Mask Expansion values are required. Click  to disable Bottom layer options if they are not required.
  • Bottom – enter the bottom layer solder mask expansion value. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. Default units (metric or imperial) are determined by the Units setting in the Other region of the Properties panel in Board mode (accessed when no objects are selected in the design space) and are used if the unit is not specified. This field is accessible only if the link icon is set to  and the Tented option is not enabled.
    • Tented – check if it desired for any solder mask settings in the solder mask expansion design rules to be overridden, which results in no opening in the solder mask on the bottom layer of this pad and is therefore tented. Disable this option and this pad is affected by a solder mask expansion rule or specific expansion value.
    • From Hole Edge – when enabled, the Solder Mask opening will follow the shape of the hole. The mask is therefore independent of pad shape and size and is scaled from both the hole size and shape. For example, a pad with a square hole will create a square mask opening that matches the hole dimensions, as well as the assigned expansion value. Also note that a pad's expansion mask opening size will track any changes in the hole size.

Testpoint

• Fabrication/Assembly – these options allow you to specify pads (thru-hole or SMD) to be used as testpoint locations in fabrication and/or assembly testing. Enable Top for this pad to be defined as a top layer testpoint. Enable Bottom for this pad to be defined as a bottom layer testpoint.