Get email delivery of the Cadence blog featured here
If you are a PCB designer and follow IPC-2581 guidelines to design a board, this solution is for you!
To ensure on-time and quality fabrication, it is essential that your design team conveys the design data not only correctly, but intelligently to manufacturers. Traditional methods of passing design information to manufacturers are prone to loss of data since there is no built-in mechanism to save the data with the design itself. But, if your designs support IPC-2581, this is no longer a problem. You can leverage the capability of the IPC-2581 data exchange format to pass the design intent to the fabrication, assembly, and testing teams for the successful manufacturing of your final product. This approach lets you incorporate design-critical information that can be revised and reused.
Use the IPC-2581 Spec element to create and assign notes, instructions, and drawings for the fabrication and assembly processes. Allegro PCB Editor provides the ability to specify these notes as IPC-2581 spec elements and associate them to a board design or to one or more objects of a design. These specs created in the IPC-2581 format include high-levels of accuracy and details that can be used in post-design processes.
IPC-2581 Spec is an XML element within the IPC-2581 manufacturing data file. It is used to assign different attributes to graphical and electrical elements of a design. A spec may contain one or more entries to cater to different requirements. For example, the first entry contains a fabrication note, the second defines an assembly instruction for a part, and the third specifies the impedance value for clines. The spec becomes part of the IPC-2581data and is directly read by an IPC-2581 viewing tool, eliminating the need for a separate utility to access the required information. Once you have created the specs, export to a SPEC template so that other designs can import the template – that’s reuse!
Before attaching specs to database objects, you first need to define them. Simply choose Setup – IPC2581 Spec Definition or type define ipc spec in the command window to open the Define IPC2581 Specs dialog box and then specify a name and select design elements for which the spec is being created, followed by the type and subtype.
Once done, click Add and enter the details either as text strings or as numerical values. You can modify these details saved as spec properties anytime you want.
If you want to reuse the Spec, say to ensure the consistency of messages across multiple designs, save the spec definitions in an XML-formatted configuration file at the location specified by the ipc2581spec_path environment variable by clicking Export in the Define IPC2581 Specs dialog.
Once defined, attach these specs to objects in a design. Just choose Edit – IPC2581 Specs or enter ipc spec edit in the command window and enable objects in the Find filter. This opens the Edit IPC2581 Specs window where all the specs are listed, which can be applied to the selected object. Select the spec and apply it to the required object.
Now, you might want to include the spec assignments when exporting IPC-2581 data for a design; go ahead and set the environment variable ipc2581_export_user_specs in the User Preferences Editor. That will do it.
If you want to use this solution but wish to first run through the steps using a sample design, try out the steps explained in the Rapid Adoption Kit on IPC-2581 SPECs in PCB Editor. This RAK has a sample design database and detailed step-by-step instructions that will help you understand the functionality in no time.