Pad

Old Content - visit altium.com/documentation

Modified by Admin on Nov 6, 2013

The Bottom Layer Dialog.

Summary

This dialog allows the designer to specify the properties of a Pad.

Access

The pad dialog can be accessed prior to entering placement mode, from the PCB Editor - Defaults page of the Preferences dialog (DXP >> Preferences). This allows you to change the default properties for the object, which will be applied when placing subsequent Objects.

During placement, the dialog can be accessed by pressing the Tab key.

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

Double-clicking on a placed Pad.
Placing the cursor over a Pad, right-clicking and choosing Properties from the context menu.
Run command Edit >> Change, then click an existing object.

Options/Controls

Location

X - The 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 values can be entered in either mm or mil units. To specify the units when typing a number, add the mm or mil suffix to the value.Y - The field shows the current Y position of the center of the pad relative to the current origin.
Edit the values in these fields to change the position of the pad relative to the current origin. The values can be entered in either mm or mil units. To specify the units when typing a number, add the mm or mil suffix to the value.
Default units (metric or imperial) are determined by the Units setting in the Board Options dialog (Design >> Board Options), and are used if no units are specified.
Rotation - This field shows the current pad anti-clockwise rotation in degrees. Edit this field to change the rotation of the pad. Minimum angular resolution is 0.001°.

Hole Information

Hole Size - The field shows the current hole size for the pad. The value specifies the diameter of the hole (as a round, square or slotted shapes), 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. Values can be entered in either mm or mil units. To specify the units when entering a number, add the mm or mil suffix to the value.
Default units (metric or imperial) are determined by the Units setting in the Board Options dialog (Design >> Board Options), and are used if no units are specified.
Round - Specifies a round hole shape (default) for the hole size of a pad. Separate drill file (NC Drill Excellon format 2) are generated for each hole kind (round, square and slot) as well as for plated and non-plated holes. There are up to six different drill files for these types.
Square - Specifies a square (punched) hole for this pad and specify the rotation of the square holes. Square holes can be plated or unplated. Separate drill file (NC Drill Excellon format 2) are generated for each hole kind (round, square and slot) 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 and then specify the length and the rotation of the slot. Slotted holes can be plated or unplated. Separate drill file (NC Drill Excellon format 2) are generated for each hole kind (round, square and slot) as well as for plated and non-plated holes. There are up to six different drill files for these types. If enabled, two new fields will appear, Length and Rotation.
- Length - Shows the current round ended slot length for the hole of the pad. The value specifies the length of the slot 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 this field to change the slot length. Values can be entered in either mm or mil units. To specify the units when typing a number, add the mm or mil suffix to the value.
  Default units (metric or imperial) are determined by the Units setting in the Board Options dialog (Design >> Board Options), and are used if no units are specified.
- Rotation - Shows the current slot hole's anti-clockwise rotation in degrees. Edit this field to change the rotation of the slot. Minimum angular resolution is 0.001°.

Properties

Designator - This field shows current pad designator. If the pad is part of a component, the designator is usually set to the corresponding component pin number. The designator can be up to 20 characters in length and cannot include any spaces. 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 shows the layer the pad is currently assigned to. 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 - This field displays the net that the pad is currently assigned to. Change the net assignment by clicking in the field and choosing a net from 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.
Electrical Type - This field shows 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.
Plated- This option determines whether or not the pad has a plated hole. A check mark 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.
Click the checkbox to toggle the option on or off.
Locked- Enable to protect the pad from being edited graphically. Lock a pad whose position or size is critical. If you try to edit a primitive that is locked, you will be informed that the primitive is locked and asked if you wish to proceed with the action. If this option is unchecked, the primitive can be freely edited without confirmation. If this option is disabled, disable the top or bottom test point options to unlock this pad.
If the Protect Locked Objects option is enabled in the PCB Editor - General page of the Preferences dialog (DXP >> Preferences), and the Locked option for this pad is enabled as well, then it cannot be moved.
Jumper ID - Use this field to provide 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 ID value tells Altium Designer which pads to treat as 'connected'. A jumper connection can only be created amongst the pads within a component footprint. The pads used must use the same Jumper ID value and must also share the same net. A jumper connection is shown as a curved connection line in the PCB Editor.

Testpoint Settings

The designer can specify testpoint settings for Fabrication or Assembly.

Top - A test point is a location where a test probe can be connected to the PCB to check for correct function of the board. Any pad or via can be nominated as a top layer or bottom layer test point and this pad / via gets locked.
The Find and Set Testpoints feature can be used to search for existing pads and vias that can be used as testpoints. Defining the properties of pads and vias that can be used as Testpoints is done by configuring the Testpoint Style design rule. Enable this option if a pad is to be nominated as a top layer test-point.
Bottom - A test point is a location where a test probe can be connected to the PCB to check for correct function of the board. Any pad or via can be nominated as a top layer or bottom layer test point and this pad / via gets locked.
The Find and Set Testpoints feature can be used to search for existing pads and vias that can be used as testpoints. Defining the properties of pads and vias that can be used as Testpoints is done by configuring the Testpoint Style design rule. Enable this option if a pad is to be nominated as a bottom layer test-point.

Size and Shape

Simple - Enable this option to select a simple layered pad. You can define X and Y sizes and shape attributes which are common for all layers of this pad.
Top-Middle-Bottom - Enable this option to select a Top-Middle-Bottom layered pad object. You can define X and Y sizes and shape attributes for top, middle and bottom layers respectively for this pad object.
- X-Size - Shows the current X (horizontal) size of the pad. The X and Y (vertical) values set the size of the pad can accept values of 1 to 10000mil. The X and Y size can be set independently to define asymmetric pad shapes.
  Edit these fields to change the pad size. Values can be entered in either mm or mil units. To specify the units when typing a number, add the mm or mil suffix to the value. Y-Size - Shows the current Y (vertical) size of the pad. The X (horizontal) and Y values set the size of the pad can accept values of 1 to 10000mil. The X and Y size can be set independently to define asymmetric pad shapes.
- Edit these fields to change the pad size. Values can be entered in either mm or mil units. To specify the units when typing a number, add the mm or mil suffix to the value.
  Default units (metric or imperial) are determined by the Units setting in the Board Options dialog (Design >> Board Options), and are used if no units are specified.
- Shape - This field shows the current basic pad shape. Basic pad shapes include Round, Rectangular, Octagonal, Rounded Rectangle.
  Basic shapes can be manipulated by changing the X and Y size settings to produce asymmetrical pad shapes. To change the pad shape, click on the field and select an option from the dropdown list: Round, Rectangular, Octagonal, Rounded Rectangle.
- Corner Radius - Represents the corner radius of a pad. Pad radius is represented as a percentage of half of the shortest side of the pad. As such, a value of 0% corresponds to a rectangular pad, and 100% to a circular pad. This field only applies when the Shape field is set to Rounded Rectangle.
  To change the corner radius, click in the field and enter a new percentage. The X (horizontal) and Y (verical) sizes can be set independently to define asymmetric pad shapes.
- Offset From Hole Center(X/Y) - Enter a value to offset the pad landing area from the center of the pad hole.

Paste Mask Expansion

Expansion value from rules - Enable this option to allow the existing paste mask expansion rule to take effect on this pad object. Check the Mask design category from the PCB Rules and Constraints Editor dialog.
Specify expansion value - Enable this Specify expansion value option to edit the expansion value and the paste mask expansion design rule is overridden for this pad.

Solder Mask Expansions

Expansion value from rules - Enable this option to allow the existing solder mask expansion rule to take effect on this pad object. Check the Mask design category from the PCB Rules and Constraints Editor dialog.
Specify expansion value - Enable this Specify expansion value option to edit the expansion value and the solder mask expansion design rule is overridden for this pad.
Force complete tenting on top - Enable the Force complete tenting on top option and any solder mask settings in the solder mask expansion design rules will be overridden and results in no opening in the solder mask on top layer of this pad.
Disable this option and this pad is affected by a solder mask expansion rule or specific expansion value.
Force complete tenting on bottom - Enable the Force complete tenting on bottom option and any solder mask settings in the solder mask expansion design rules will be overridden and results in no opening in the solder mask on the bottom layer of this pad.
Disable this option and this pad is affected by a solder mask expansion rule or specific expansion value.