BoardSurfers: Detect Missing Padstacks Masks Using Allegro X PCB DesignTrue DFM

A common Design for Manufacturing (DFM) mistake that could lead to rework when designing a PCB is the oversight of padstack masks. When defining libraries, it is essential to specify soldermask and pastemask for surface mount pads, as well as soldermask for through-hole pads. Mask layers often get missed when creating footprints due to human error. Additionally, manually probing padstacks for masks or visually verifying their existence can be prone to mistakes and is time-consuming, especially when verifying multiple padstacks in a PCB design. However, these missing masks can be quickly and easily identified using Allegro X PCB DesignTrue DFM constraints. You can set these constraints in either the Symbol Editor or PCB Editor.

Effects of Missing Solder and Pastemasks

When soldermask definitions are missing from padstacks, the pads become completely covered by the soldermask. As a result, components cannot be properly soldered onto the PCB. Similarly, if the pastemask is not defined in the padstack, you cannot apply solder to the surface-mounted (SMT) components while assembling the PCB.

Setting DFM Constraints for Missing Masks

DesignTrue DFM (Design for Manufacturing) constraints can help identify missing masks during the library creation stage or at any later stages of the design process. These constraints can also be exported when developing new PCBs to identify any missing masks.

Before adding DFM constraints, ensure that you define the mask layers in the Cross-Section Editor, as illustrated in the following image:


For more information, watch the video on How to Add Non-Electrical Layers to the Stackup to Enable the Non-Electric Layer DFM Check.

Enabling Constraint Modes

To enable constraints for missing masks in the Symbol Editor or PCB Editor, choose Setup – Constraints – Modes. In the Analysis Modes dialog box that opens, navigate to Design for Fabrication – Annular Ring. Then, select the checks for missing masks related to pins and vias, as shown in the following image:

Similarly, navigate to Design for Assembly– Pastemask and select the Missing pastemask check box:

Click OK to close the Analysis Modes dialog box to apply the changes you made.

Creating Constraint Sets for Missing Solder and Pastemasks

To set constraints for missing soldermasks, follow these steps:

1. Select Setup – Constraints – Manufacturing.
   Constraint Manager opens.
2. Navigate to Design for Fabrication – DFF Constraint Set and select the Annular Ring worksheet.
3. Click the cell labeled <Create new> under the Name column. Specify a name for the constraint set, such as Missing Solder.
4. Set the CSet Usage as Non-Etch and click Ok.
   
5. Set the Missing mask constraint value to On for all pins and vias using the pull-down options, as illustrated in the following image:
   
   

For missing pastemasks, follow these steps:

1. Navigate to Design for Assembly – DFA Constraint Set and select the Pastemask worksheet
2. Click the cell labeled <Create new> in the Name column
3. Specify a name for the constraint set, such as Missing Paste
4. Leave the CSet Usage value unchanged and click Ok
   By default, it is set to Non-Etch
   
   
   
5. Set the Missing pastemask constraint value to On using the pull-down options as shown:
   

The necessary constraints are in place for both solder and pastemasks.

Assigning the Constraint Set

After creating constraints, assign them to the design. To do this, navigate to Design for Fabrication – Design – Annular Ring and assign the Missing Solder CSet to both, the soldermask top and bottom layers.


Similarly, assign the Missing Pastemask CSet to the pastemask layer in Design for Assembly – Design– Pastemask.

Finding and Resolving Missing Masks DRCs

Once the constraints are assigned, choose Tools – Update DRC to generate Design Rule Check (DRC) errors for missing solder and pastemasks. Select a DRC error and select Display – Element to view its details.

After identifying the padstacks with missing solder and pastemasks, follow these steps to resolve the DRCs:

1. Choose Tools – Padstack – Modify Design Padstack
2. Select a padstack in the design canvas, right-click, and choose Edit
   Padstack Editor opens with the selected padstack data
3. Add the necessary mask layers for the selected pad
   
4. Choose File – Update to Design to save the padstack updates
5. Choose Exit to close the Padstack Editor
6. Continue editing padstacks with missing mask layers
7. Select Tools – Update DRC to verify whether the DRCs are resolved
   

The Export and Import options in Constraint Manager enable the export of the manufacturing constraints for missing masks to other designs. For more information, watch the video titled Using Constraint Files to Re-use Design Data within the PCB Editor available in the Allegro X PCB Editor Intermediate Techniques Course – Video Channel.

Some designs use tented vias, which are covered by a soldermask or similar material on both sides of the PCB. In such designs, you can ignore certain padstacks while checking for missing masks. To learn how to exclude specific padstacks while performing missing masks checks, refer to this video: How to Identify missing soldermask and pastemask in padstacks using Allegro X DesignTrue DFM.

Conclusion

Using Allegro X DesignTrue DFM for detecting missing padstack masks significantly streamlines the PCB design process, minimizing the risks associated with manual oversight. By effectively setting and managing DFM constraints, you can proactively address potential issues before they manifest, saving time and reducing rework. The ability to quickly identify and resolve missing mask definitions ensures a smoother assembly process, enhancing the overall quality and reliability of the final product. If you want to deepen your understanding of DFM practices, you can enroll yourself in the Allegro X DesignTrue DFM Training course.

Contact Us

For any feedback or topics that you want us to include in our blogs, write to us at pcbbloggers@cadence.com.
Subscribe to stay updated about our upcoming blogs.

About BoardSurfers

The BoardSurfers series provides solutions to the various tasks related to the creation and management of PCB design using the Allegro X platform products. The name and logo of this series are designed to resonate with the vision of making the design and manufacturing tasks enjoyable, just like surfing the waves. Regular, new blog posts by experts cover every aspect of the PCB design process, such as library management, schematic design, constraint management, stack-up design, placement, routing, artwork, verification, and much more.