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 IPC Compliant Footprint 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 PCB Component 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 PCB Component Wizard you enter the sizes required for the pads and component overlay.
To launch the PCB Component Wizard, right-click on the Footprints section of the PCB Library panel then select Footprint Wizard or select the Tools » Footprint Wizard command 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.
If only pad objects have been used to build up an irregular shape, the matching irregular mask shape will be generated correctly. 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 handled manually.
Manually applying solder and paste mask expansions can be achieved by placing lines (tracks), fills, regions, or arc primitives on the corresponding solder or paste mask layer. You can then make use of the Solder and Paste Mask Expansion settings within the primitives used to create the irregular pad shape.
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 top of 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 circle shown behind the two sets of fingers. Each set of copper fingers has been defined by an arc, horizontal lines, and a pad. The pads are required to define the points of connectivity. Manually placed solder mask definitions will automatically be transferred to the bottom side solder mask layer when the component is placed on the bottom of the board.
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 peelable 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.
After completing the creation of a PCB Footprint, the footprint and any additional 3D model/body information (all of which comes together to create the component model) can be released to and stored in a server. A server-based component gathers together all information needed to represent that component across all design domains within a single entity. It could, therefore, be thought of as a container in this respect. A 'bucket' into which all domain models and parametric information is stored.
In terms of its representation in the various domains, a server-based component does not contain the domain models themselves, but rather links to these models. These links are specified on the design side, as part of the source component definition from which the released Component Item is generated. As such, before you can delve into the process of defining and releasing server-based components, you must first ensure that all the domain models themselves have been created and released.
Please Complete the form below to get Free Trial of Altium Concord Pro