Materials are critical for manufacturing a reliable PCB or package design. The performance, shelf-life, and cost of a PCB or package is determined by the materials used in its stackup. Choosing the right materials is essential to ensure the intended functionality of the final product.

Allegro® platform applications provide an easy-to-use tool to select and manage materials right from the outset. This tool is called Material Editor and is accessible through all Allegro platform PCB, Simulation, and Packaging applications. It uses a common material file material.cmx, which is read by Allegro® PCB Editor, Allegro® Package Designer Plus, and Sigrity simulators. It is pretty simple to define and manage materials using Material Editor. 

Setting-up Materials

In a new design, you can assign materials using the Setup ─ Materials option inside Allegro PCB Editor or Allegro Package Designer Plus.

For managing materials, the Materials Editor interface supports a single file (material.cmx) that records material information such as, material name, type (dielectric or conductor), thermal and magnetic models, temperature and frequency-specific dielectric models, temperature specific metal conductivity, and so on. This information is utilized for simulation in the Sigrity simulators. For example, the Design column categorizes materials specific for PCB or package.

Materials Editor, by default, displays the metal conductivity defined at 20C. You can modify this value by selecting the conductivity cell for any material. A sub-dialog is provided to view or edit the temperature-specific conductivity. The value at 20C is also considered in Cross-section Editor. In the following example, conductivity of SILVER is defined at different temperatures, but both Material Editor and Cross-section Editor display the value 6.3e + 0, which is the value at 20C.

If no conductivity value is defined at 20 C for any material, the first row is displayed irrespective of the temperature value. For example, SOLDER60 has conductivity values defined at 25 C and 35 C. In the Material Editor, only the first value is displayed along with its temperature. Cross-section Editor also picks the first value and displays it.

Similarly, the values of Dielectric Constant and Loss Tangent are also defined for 20C at 1000Mhz frequency. The same value is read in Cross-section Editor.

Any edits of the material properties are stored directly in the design database irrespective of the application you are using. The same material.cmx file is used from the library for other materials. Since the edited values are stored in the design database, the overridden values are read from the database and are displayed in bold-blue color. In the following image, you can see that for 1OZ_Copper, the Thickness is modified and hence the complete row is displayed in bold-blue indicating that the values were edited and are not the default values.

Any mismatch in values between Cross-section Editor and Material Editor is reflected in bold-blue color. You can see that for Copper the default value of conductivity in Materials Editor is 5.96e+07 mho/m @ 20 C, but the Cross-section Editor has a value of 595900 mho/cm. Therefore, this value is displayed in bold-blue color.

Refreshing the values in Cross-section Editor from Materials Editor clears the override and the value is displayed in the default font style and color.

Note that values for electrical conductivity are now in mho/m as opposed to mho/cm in legacy Material Editor.

Exporting Materials for Reuse

Legacy Material Editor used to save edits in separate files (materials.dat or mcmmat.dat) on disk at the design-level and these files were used as default materials files. While the new Material Editor, available with release 17.4, saves all the edits in materials directly in the design database as overrides. So, if you want to reuse edited materials in any other design, simply export the materials using the File ─ Save As option and use the same material.cmx file.

Migrating Legacy Materials Files to New Format

A legacy material file (materials.dat/mcmmat.dat) can be imported in the Materials Editor to create a new material.cmx. On importing, contents of materials.dat are merged with the library defined for material.cmx file.

1. Open Material Editor and choose File ─ Incremental Merge.

2. Read the message and Click OK to close the message dialog.

3. Select the file-type as Legacy Materials Files (*.dat) and browse the file.

New materials and materials with modified values are displayed as overrides in bold-blue.  

4. Choose File ─ Save As and save the file with the extension .cmx.

    Note: To set .cmx as default materials file, open User Preference Editor and set the value of the MATERIALS_PATH environment variable to the path of material.cmx.

Any custom materials.dat exists and is specified as MATERIALS_PATH value will be preferred and used as the default materials file.

Conclusion

Whether you are working with Allegro PCB Editor, Allegro Package Designer Plus, or Sigrity simulators, there is always a need to tweak the material properties to accomplish the intended results. Legacy material editors supported different file formats leading to inconsistencies across PCB and package substrate design applications. This drawback due to inconsistency is now overcome by the new Material Editor that uses a common material file in all the applications. Any edits to this file are saved in the database and can be leveraged in future designs just by exporting the material file.