Связаться с нами
Связаться с нашими Представительствами напрямую
The real-world component that gets mounted on the board is represented as a schematic symbol during design capture, and as a PCB footprint for board design. Altium Designer components can be:
The typical sequence for manually creating a component footprint is:
.Commentspecial strings on a mechanical layer.
The IPC Compliant Footprint Wizard creates IPC-compliant component footprints. Rather than working directly from footprint dimensions), the Wizard uses dimensional information from the component itself then calculates suitable pad and other footprint properties in accordance with the algorithms released by the IPC.
Some of the IPC Compliant Footprint Wizard features include:
The IPC Footprint Batch Generator can be used to generate multiple footprints at multiple density levels. The generator reads the dimensional data of electronic components from an Excel spreadsheet or comma delimited file then applies the IPC equations to build IPC compliant footprints. Support for the IPC Footprints Batch Generator includes:
\Templatesfolder in the Altium Designer installation.
The PCB Library 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, right-click in the Footprints section of the PCB Library panel then select Footprint Wizard or select Tools » Footprint Wizard from the main menus.
A 3D representation of the component can be included in the footprint. The following 3D model formats can be used in Altium Designer:
The shape can be created by placing a number of Altium Designer 3D Body objects to build up the shape by placing one 3D Body object and importing a 3D model into it or a combination of both.
Some footprints require pads that have an irregular shape. This can be done using any of the design objects available in the PCB Library Editor, but when doing this, there is an important factor that must be kept in mind.
Altium Designer automatically adds solder and paste masks to pad objects based on their shape. Default expansion values are defined by design rules by default, although they can also be specified by the Pad settings contained on the PCB Editor - Defaults page of the Preferences dialog. These settings can be overridden during placement or after placement through the Properties panel.
Main article: Working with Custom Pad Shapes
If only pad objects have been used to build up an irregular shape, the matching irregular mask shape will automatically be generated as an expansion of the pad shape. But if the irregular shape was built up using other objects, such as lines (tracks), fills, regions, pads, vias, or arcs, the solder and paste masks will need to be configured manually.
All object-kinds have a solder mask property, and fill and region objects also have a paste mask expansion property. If these objects have been placed on the top layer to create a pad shape, then the solder mask property of those objects can be enabled to either obey the applicable design rule, or use a manual expansion value. If fill and region objects have been used to build up a pad shape, then the paste mask can also be enabled as a property of the extra objects.
When the mask shape is not correctly created as an expansion (or contraction) of the set of objects used to create the custom pad shape, then manually defined solder and paste mask expansions can be also achieved by placing lines (tracks), fills, regions, or arc primitives directly on the corresponding solder or paste mask layer. The custom button footprint shown below is an example of this.
To check that solder and/or paste masks have been correctly defined in the PCB Library Editor, open the View Configuration panel and enable the show option () option for each mask layer.
The image in the Footprints with Multiple Pads Connected to the Same Pin section below shows a PCB footprint with a purple (color of the Top Solder Mask layer) border that appears around the edge of each pad. This represents the edge of the solder mask shape protruding by the expansion amount from under the pad.
To quickly walk through layers, use the Single Layer Mode (Shift+S) in combination with Ctrl+Shift+Wheel roll.
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.
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.
The footprint shown below is the contact set for a push button switch implemented directly in the copper on the surface layer of the PCB.
A rubber switchpad overlay is placed on the PCB, with a small captive carbon button that contacts both sets of fingers in the footprint when the button is pressed to create the electrical connectivity. For this to happen, both sets of fingers must not be covered by the solder mask.
The circular solder mask opening has been achieved by placing an arc whose width is equal to or greater than the arc radius, resulting in the solid purple circle shown behind the two sets of fingers. Each set of copper fingers has been defined by an arc, horizontal lines, and a pad (selected in the image to make them visible). The pads are required to define the points of connectivity. Manually placed top solder mask definitions are automatically be transferred to the bottom side solder mask layer if the component is placed on the bottom side of the board.
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.
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.
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.
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.
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.
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 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.
In the below library footprint, the special string
.Designator has been placed on the Mechanical 2 layer.
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.
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:
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,
(which has a Voltage Rating value of 3kV).
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 (
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.
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 is determined by the Designator and Comment string Autoposition option in the Properties panel. The default position and size of Designator and Comment strings is configured in the respective Primitive on the PCB Editor - Defaults page of the Preferences dialog.
There may be situations where additional copies of the Designator or Comment strings are required. For example. the assembly house might want a detailed assembly drawing with the designator shown within each component outline, while in-house company requirements stipulate 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 for the assembly house's requirements, the
.Designator string would be placed on a mechanical layer in the library editor and print outs that included this layer could then be generated as part of the design assembly instructions.
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.
The Names of Mechanical Layers can be edited directly from the View Configurations dialog by right-clicking then selecting Edit Layer.
At the simplest level of 3D representation, height information can be added to a PCB Component. To do this, double-click on a footprint in the Footprints list in the PCB Library panel to open the PCB Library Footprint dialog. Enter the recommended height for the component in the Height field.
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 and/or a STEP model to the PCB Component. Details of this will be discussed in another module.
PCB Components can be copied from other PCB Libraries and then renamed and modified within the destination library to match the specifications required. There are a number of ways to execute this function.
There are a series of reports that you can run to check that footprints have been created correctly as well as identifying which components are in the current PCB library.
The Component Rule Check report (Reports » Component Rule Check) is useful for validating all components in the current PCB library by testing for duplicate primitives, missing pad designators, floating copper, and inappropriate component references.
Including PCB Libraries as part of a Integrated Library Package provides an additional layer of validation because it allows the Design Compiler to examine the Schematic and PCB models together. This, of course, requires that a Schematic Library that matches the PCB Library exists however assuming this is the case, a range of additional checks are possible using the Error Reporting tab of the Project Options dialog.
Updating a PCB Footprint can be done in two ways: "Pushing" the PCB from the PCB Library, or by "Pulling: from the PCB Editor. Pushing a PCB Footprint update takes a selected footprint(s) from the PCB Library and uses it to update all open PCB documents containing that footprint. This first method is the best option when a complete replacement is desired. The second option allows you to review all the differences between the existing footprint and the footprint in the library before the update is performed. You can also select which objects are to be updated from the library. This second method is the best option when you need to figure out exactly what has changed between the footprint on the board and the footprint in the library.
From the PCBLIB Editor, use the Tools » Update PCB with Current Footprint or Tools » Update PCB With All Footprints command. From the PCB Library panel, right-click in the Components region of the PCB Library panel then select Update PCB with [Component] or Update PCB with All. Running these commands opens the Component(s) Update Options dialog from which you can select the primitives/attributes to be updated.
A PCB 2D/3D component model can be edited and released into the initial revision of a newly-created Footprint Item through the server's support for direct editing through the Explorer panel or by using the Component Editor in Single Component Editor mode. Through direct editing, you can edit a supported Item type using a temporary editor loaded with the latest source direct from the server itself. After editing is complete, the entity is released (or re-released) into a subsequent planned revision of its parent Item and the temporary editor is closed.
Связаться с нашими Представительствами напрямую