Easier Bond Finger Solder Mask Openings

Wire bond fingers have specific requirements for exposure through the solder mask layer.


If you design wire bond packages, you’re familiar with the need for the bond fingers and rings on the package substrate layers to be exposed through the solder mask layer. If they aren’t, it becomes… rather difficult… to bond the wire to them, after all!

We talked about general-purpose bounding shapes a few weeks ago in “A Boundless Bounty of Bounding Shapes”. Bond fingers have a few specific requirements when it comes to their exposure through the solder mask layer.

When you pick up the latest hotfixes of Allegro 17.4, Hotfix 005, you’ll notice an additional option to pick the reference pad to be used for the convex hull generation – use the regular metal pad OR use the solder mask pad defined in the finger’s padstack. This request came to us recently from one of you. While we don’t make a general practice of putting enhancements into the tool in hotfix patches, we do sometimes make exceptions as we did here. As it may help others of you who organize your design data in a similar fashion, I wanted to make you aware of it.

The form – updated

The best place to start is what you’ll notice in the UI for the command. The change is minor – one new checkbox, in fact – as shown below:

Don’t worry, this won’t change your default flow if you pick up the hotfix. None of your scripts or automation will change behavior. The default for the option is disabled, meaning we will continue to measure the distance from the metal pad as in all past releases.

Why should I adjust my flow?

If you incorporate a solder mask pad in your finger definition, it can save you steps for any finger that is isolated in your pattern. You won’t need to manually add a solder mask opening around the finger, and as you move the finger during the design of your bond shell, the mask opening will automatically move along with it.

However, when you have multiple fingers together on the same path, the solder mask pads end up overlapping, as in our example below:

The overlapping of these masks is not what you want, nor are the sharp points where the arcs on the top and bottom sides intersect each other. These are points of concern during the manufacturing process. The sharp points can make it easier for the solder mask material to peel back and expose areas of the top metal layer you didn’t intend.

Therefore, the finger solder mask tool exists – to create a single, smooth opening around the pads. The mask is there to expose the conductor metal pads, not the solder mask pads we see in yellow above. If you don’t have a mask pad predefined, then you will specify the clearance to the metal pad based on manufacturing requirements. Only the one mask shape will exist in the design, and there will be no issue.

But in cases where you DO have the padstack mask pad, it already defines the ideal clearance required to the metal pad. All you’re really trying to do is create a smooth opening with no acute angles, no weak points that might compromise the intended design geometry.

With the new option turned on, give a clearance value of 0 (since the padstack pad’s already the right clearance!), and window the pads. You will get an additional shape as shown here:

Hopefully, you notice that the mask doesn’t expose any more of the pads than the individual mask pads did. All it has done is removed the intents where they overlap. We’re left with a clean, smooth opening exposing all three of our pads.

Can’t I just enter the values myself?

You certainly can! But, why? You could have different mask pad sizes for different fingers across your design for some reason, making the creation of the general mask oversized for any with smaller clearances. Even if you don’t, you need to remember the mask clearance value as given in your constraints instead of just entering zero.

Finally, there are manufacturing checks in place in the tool for validating your solder mask openings. These rules specify the minimum separation between mask openings. If you have two openings which touch, they violate this gap.

The DRC will be suppressed if there’s a mask opening completely containing the two masks (since, upon merging all mask openings together, the two smaller openings are “ignored” because of the larger opening). But, if the mask isn’t COMPLETELY contained within the larger opening, then the violation cannot be ignored. You, as the designer, must manually waive the violation after determining if the overlap doesn’t result in any undesirable angles.

This can become a problem with openings based on oversizing the metal pad because of the need to snap the points of the mask opening to your manufacturing grid. The arcs of your padstack mask snap differently than the convex hull mask. Any minute overlap will result in a DRC for you to investigate, or the need to “bump up” the mask clearance in the form, exposing more metal than you want.

By basing the bond finger solder mask opening relative to the mask pads, you eliminate this because the actual pad is used. Snapping can adjust the outline and ensure no registration errors will occur. Meaning that not only do you not have to remember the spacing values, you don’t need to check and waive any DRCs, either!

Try it for yourself!

The only certain way to determine if this will make your design process simpler is to try it yourself. If you agree, as we do, that this makes your life easier, thank your fellow users for the wonderful recommendation!

Leave a Reply

(Note: This name will be displayed publicly)