Шаблоны и библиотеки контактных площадок и переходных отверстий

Along with Track objects, Pads and Vias are fundamental elements of all circuit board designs. To raise the design reuse and management capabilities for Pads and Vias in PCB designs, Altium Designer supports Pad and Via template Libraries.

The concept of Pad and Via templates that can be collected in a Library is not unlike that of PCB footprint libraries, although somewhat more basic. The Pad Via Template library does not store actual Pads and Vias, rather it stores pre-configured definitions that are applied to an instance of a Pad or Via as it is placed. Saved Pad Via Template libraries can be loaded and used to place instances of predefined Pads and Vias in any PCB design or PCB footprint.

Pad Via Template libraries are another design document that can be created in Altium Designer and have the file extension *.PvLib. Pad Via Template libraries can be included as a project document, and if so, those templates are always available to that project through the PCB Pad Via Templates panel. Template libraries can also be installed in the panel, making them available to all open projects. Learn more about making templates available on the Working with Pad Via Templates page.

Pad and Via Templates are created and edited by opening a PvLib file. The Pad and Via Templates in the PvLib are listed in the Pad Via Library panel, with the selected Pad or Via Template displayed in the Pad/Via Template Editor, as shown below.

❯ ❮ Javascript ID: PvLib_Editor

Both Pad and Via Templates are edited by opening the PvLib file. The editor options will change to suit the type of object being edited. The Pad Template Editor is shown here. Both Pad and Via Templates are edited by opening the PvLib file. The editor options will change to suit the type of object being edited. The Via Template Editor is shown here.

Creating a Pad Via Template Library

A new pad/via template library can be created by the following ways:

• Select File » New » Library command from the main menus and select the Pad Via Library option from the File region of the New Library dialog that opens, then click Create. The new Pad Via Template library is given a default name of PvLib1.PvLib. At this stage, the file has not been saved to the hard drive; it only exists in the computer memory. Because it is unsaved, the first time you save it, the Save As dialog will open, offering to save it to the Default Location defined on the System – Default Locations page of the Preferences dialog.
• A new Pad Via Template library can also be added to the current project by right-clicking on the project in the Projects panel and selecting Add New to Project » Pad Via Library from the context menu. The file will appear in the Libraries/Pad Via Library Documents folder of the project structure. When the file is saved, the location will default to the project folder.

• A Pad Via Template library can be created from the Pads and Vias in an open PCB in the Pad & Via Templates mode of the PCB panel. Using the standard Windows selection techniques, select the Pad/Via templates to be saved into the library then click the Save as Library button. The new PvLib will open ready for editing, but will not have been saved to the hard drive. Save the file to a suitable location, naming it as required. When the Pad Via Template library first opens in the Template editor it may show only one pad template in the Pad Via Library panel (the default template). If this occurs, save, close, and reopen the file to refresh the list of templates in the Pad Via Library panel.

  
  A Pad Via Template library can be created from the selected pads/vias in the current PCB.

Pad Via Library Panel

The Pad Via Library panel provides access to Templates contained in the active Pad Via Library. The Pad Via Library panel available in the pad/via template editor lists the Pad and Via templates contained in the current Pad Via Template library. The preferred units for this editing session are selected from the Display Units drop-down menu at the top of the panel.

The Pad Via Library panel

Panel Access

The panel is accessed from the Pad/Via Template Editor (having a *.PvLib document open as the active document in the design space) in the following ways:

• Click the Panels button in the bottom-right corner of the design space then select Pad Via Library.
• Click View » Panels » Pad Via Library from the main menus.

Creating a Pad or Via Template

To create a new Pad or Via template, right-click within the panel then select Add Pad template or Add Via template from the context menu. Use Delete to remove a template from the Library.

The panel provides access to Templates contained in the current Pad Via Library. Right-click to add a new Template.

Pad/Via Template Editor

The Pad Template Editor is used to configure the base configuration options for a Pad or Via template that can then be applied to a Pad or Via in a PCB or PCB footprint document. These include the main properties of a Pad/Via configuration, while document-specific properties are (such its position, orientation, layer, etc.,) are defined when the Pad or Via is placed in a design document.

The Template editor is used to configure the Pad or Via template currently selected in the Pad Via Library panel.

The majority of Pad/Via configuration options are standard and familiar Altium Designer Pad and Via settings (Size, Hole and Mask, etc.). The Pad Template editor shares a common interface design and many of the options with the Via Template editor. Each region of the template editor is described below, with the options that are specific to Pads or Vias marked as such.

General

• Name – defaults to an automatic name based on the pad/via attributes, in accordance with the IPC-7251/7351 Padstack naming conventions (described here). A manual name can be defined if required, and removed again by clicking the button. If a manually named template has been used in a board design and that template is then unlinked from the Template library (so its properties become editable), the manual name is replaced by the automatic name.
• Description – optional description.
• Pad Type (pad only) – Surface mount or Through hole.

Hole Information

• Hole Size – denoted by h<Value> in the name, diameter of the hole.
• Tolerance – denoted by Tol in the name, enter the + and - hole tolerances, if required. Enter N/A if not applicable.
• Hole Type (pad only) – Round, Square or Slot.
• Length (pad only) – denoted by _<Value> being appended to the Hole Size in the name, length of the Square hole or Slot.
• Rotation (pad only) – angle of rotation of the Square hole or Slot.
• Plated (pad only) – plated, or not plated (not plated denoted by n in the name).

Paste Mask (pad only)

• Manual Expansion – check the box to define a manual expansion value that will override a design rule value when the pad is placed in a PCB design. This value is denoted by p<Value> in the pad template name.
• Expansion – amount to expand (a positive value) or contract (a negative value) the opening in the Paste Mask. Could be defined as either an absolute value (mil/mm) or percentage of the pad area. When an absolute value is defined, percentage will be shown at the right of the field, and vice-versa. Uncheck the Use Paste box at the left of the field to disable use of the paste mask for the pad template.

Solder Mask

• Manual Expansion – denoted by m<Value> in the name, where m<Value> is the overall size of opening in the Solder Mask. The naming element becomes m<Value>mx<Value> if Top and Bottom expansion values are not linked.
• Top/Bottom – amount of expansion, measured from the edge of the pad/via unless the Solder mask from the hole edge option is enabled.
• – Top and Bottom values are linked (same), click to define different Top and Bottom values.
• Tented – enable to close the opening in the Solder Mask (size of opening is set to zero).
• Solder mask from the hole edge – enable to reference the expansion value from the edge of the hole, instead of the edge of the pad/via.

Via Types & Features (via only)

• IPC 4761 Via Type – use the drop-down to select a via type according to the IPC 4761 standard, Design Guide for Protection of Printed Board Via Structures.
• Grid – appears when a via type other then None is selected in the IPC 4761 Via Type drop-down. Select board Side and type in a Material for the features available according to the selected via type.

Size and Shape

• Offset From Hole Center (X/Y) (pad only) – denoted by o<Xvalue>_<Yvalue> in the name, amount that the pad hole is offset from the pad center.
• Mode – type of pad/via-stack, options include Simple, Top-Middle-Bottom, or Full Stack (for pads this option is available only when the Pad Type is Through hole). Allows pads/vias to have different Size and Shape properties on the layers made available for that mode. Naming element x<Xvalue_Yvalue> added when a different size/shape is defined for the Bottom layer. Naming element z<Xvalue_Yvalue> added when a different size/shape is defined for mid layers. 
• Attributes on Layer – standard pad/via attributes.
  • Shape (pad only) – denoted by c<SizeValue> (circular); s<SizeValue> (square) or r<xSizeValue_ySizeValue> (rectangular) depending on if X/Y dimensions are the same or different; s<SizeValue>c<Value> (octagonal); s<Sizevalue>r<Radius%Value> or r<xSizeValue_ySizeValue>r<Radius%Value> (rounded rectangle).
  • X & Y Size (pad only) – dimension of pad in the X & Y plane.

  • Corner Radius (pad only) – absolute value of the pad corner radius. The value must be less than or equal to half of the shortest pad side. Enter a value followed by the % symbol to define the radius as the percentage of half of the shortest pad side, where 100% completely rounds the shortest pad side. This option is accessible only if Rounded Rectangle is selected for the pad Shape.

    The ability to define the corner radius as an absolute value is available when the PCB.Pad.CustomShape.CornerRadiusAbsolute option is enabled in the Advanced Settings dialog. When this option is disabled, the value in the Corner Radius field can only be defined as a percentage of half of the shortest pad side.
  • Diameter (via only) – diameter of the via (vias can only be circular).
• Thermal Relief – thermal relief settings from this pad to a surrounding polygon of the same net, clear the From Rule checkbox to edit and use these local settings.
  • From Rule – local settings are not applied when this option is enabled, clear to set and use local settings.
  • Connect Style – style of thermal relief.
  • Air Gap – distance from the pad edge to the surrounding polygon.
  • Conductors – number of conductors from the pad to the surrounding polygon.
  • Width – width of the conductors from the pad to the surrounding polygon.
  • Angle – angular pattern of the relief conductors.
• Layer – layers in this padstack/viastack, available layers depend on the current Mode setting; right-click to Add, Remove or Reset the layers when Mode is Full Stack.