BoardSurfers: Exchanging Manufacturing Data in IPC-2581 Format Using Allegro PCB Editor

15 Jul 2021 • 6 minute read

The PCB manufacturing industry has been using the Gerber data format for decades for transferring PCB design files to manufacturers. Though the Gerber format has improved over the years, it still lacks the intelligence to accurately convey the design intent. As an alternative to Gerber, the IPC-2581 data format was developed in 2004. IPC-2581 ensures efficient PCB design data transfer and brings advanced capabilities to extract all the required data for manufacturing and assembly. This includes netlist, test pad information, artwork, drill data, bill of materials, test files, and design variants. While exporting data, you can choose to suppress any information which is not needed for fabrication, assembly, testing, or procurement. You can share the design data with the manufacturing team for quick Design for Manufacturing (DFM) checks and incorporate their feedback in real-time to save you time and effort.

What is IPC-2581

IPC-2581 is a generic standard for PCB and assembly manufacturing data and transfer methodology. This standard synthesizes all aspects of a design into one XML file. The format of this file is defined and maintained by a consortium of PCB manufacturers and suppliers. Cadence is a founding member of the IPC-2581 consortium. For more information, visit the Cadence IPC-2581 link.

In this blog post, we will explore how to export and import IPC-2581 files using Allegro® PCB Editor. The advantage of using Allegro PCB Editor is that it provides a user interface with multiple pre-configured fields that help you customize your data for exporting. Depending on the recipient, you can configure these fields so that only relevant information is conveyed. That way, you can transfer the data necessary for the external partners and protect the design IP. The output is generated as a single XML file containing all the specific details. You can send this file to manufacture or assembly counterparts for evaluation during any time of the design cycle. Since it follows an XML schema, the file is readable and easy to comprehend by designers and manufacturing experts. It can be uploaded directly into the manufacture’s CAM tools and interpreted accordingly without needing any conversion program. The manufacturing experts can relay their feedback through the same XML file, which you can import into the design. Before implementing the feedback, you can compare the original IPC-2581 file with the one you received. The differences in the design are displayed in the UI. The entire process is completely automated and does not require any manual intervention at all.

Let’s go through the process of exporting and importing IPC-2581 data in detail.

Exporting Manufacturing Data into IPC-2581 Format

Extracting manufacturing data from a design in Allegro PCB Editor in the IPC-2581 format is a simple procedure. Let’s say your layout design is almost ready. At this stage, you can send the design data to manufacturers so that they can run quick DFM checks and provide some feedback before you finalize routing and placement. To generate that data in the IPC-2581 format, first launch the IPC2581 Export form and configure the options or use the default settings.

Choose File – Export – IPC2581.

The IPC2581 Export form is displayed.

Specify a name for the output file. By default, it takes the name of the current design.
Choose a version that is supported both at your end as well as by your manufacturing facility.

You can choose from the four available options: 1, A, B, or C. IPC2581-B is the most widely used version, while IPC2581-1 and IPC2581-A are obsolete. IPC2581-C is the latest and the highest version and includes additional features, such as support for rigid-flex, embedded components, cavities, edge plating, and countersink/counterbore backdrill.

The Output units field shows the current units for the active design.

You can choose to save information in a different unit in the output XML file.

Select FABRICATION as the Functional Mode.

When you select a functional mode, the default options available for the relevant attributes or functions are automatically selected in the File Segmentations and Function Apportionment section. You can also choose more options to include additional information in the XML file.

The functional mode represents data extraction types defined in the IPC-2581 standard. For versions earlier or lower than IPC2581-C, you should select both Functional Mode and Function Level to specify the data type to be extracted. Using functional modes, you can also export BOM, electrical data, layer information, and so on.

To create or edit the artwork details, click Film Creation.

The Artwork Control Form is displayed.

Click the Domain Selection button to open the Film Domain Setting form. Verify that the IPC2581 column is enabled for the artwork films you want to export and close the form.

When exporting data with the IPC2581-C version, you can modify a layer name in the exported file by adding filename affixes to the non-conductor artwork film names. To add global film filename affixes in the General Parameters tab, you need to set the ipc2581_enable_artwork_filename_affixes environment variable in the User Preferences Editor.

To map film records to specific layer types expected in the IPC-2581 file, click the Layer Mapping Edit button in the IPC2581 Export form.

IPC2581 Layer Mapping Editor is displayed. The layers are already enabled based on the layer naming settings in Artwork Control Form. You can customize this information for Inner Copper, Outer Copper, Documentation, Solder Mask, Solder Paste, Silkscreen, or Fab Layers in this form.

To include component or net properties in the IPC-2581 file, open the Export Property tab to add properties.
Close IPC2581 Layer Mapping Editor.
Click Export to generate the IPC-2581 file.

You can send the generated IPC-2581 file to the manufacturing facility to run DFM checks on the design data.

Here is a sample IPC-2581 file created for sharing fabrication data.

Importing IPC-2581 File

The same XML file can be used by the manufacturer to share feedback. When imported back into the design, this file creates new Manufacturing subclasses by adding the IPC prefix to the film record name. By comparing film records you can view the updates suggested by the manufacturer.

You can import the file using a simple GUI that provides an option to visually compare the design changes. To launch this GUI:

Choose File – Import – IPC2581.

Browse to the IPC2581 (.xml) file received from the manufacturer.
Enable the Layer stackup option to import stackup details in your design.
Click Import to start the import process.

After the import process is completed, the Compare and Purge Import options are enabled.

Click Compare to view the layer-wise differences between the original and the imported film records.

The IPC2581 Compare form is displayed. You can toggle the visibility of IPC2581 layers and artwork film names and compare the artwork data.

To compare an IPC layer with a different layer of Film, modify the mapping by clicking the ellipses for the layer. For example, the IPC_Bottom can be compared with any layer selected from the drop-down menu in the Select film to map dialog.

The Purge Import option, as its name suggests, removes imported data from the design.

View the IPC-2581 video for a quick view of the steps explained in this post.

In the End

Leveraging the capabilities of the IPC-2581 data exchange standard accelerates manufacturing and assembly and improves the turn-around time of complex designs. Allegro PCB Editor is equipped with all the features that help you exchange the intended manufacturing details with your manufacturing partners. The responsive and agile GUI-based environment aligned with IPC releases ensures the delivery of high-quality products in reduced time.

Do SUBSCRIBE to be updated about upcoming blogs. If you have any topic you want us to cover or any feedback for us, you can write to us at pcbbloggers@cadence.com.