We're in the process of building a prototype Gigabit Ethernet daughter card to evaluate Texas Instrument's DP83867CS device. This device is packaged in a 7 mm2 48-pin QFN package with a 4.1 mm2 thermal pad. Although BTC's are very popular devices, creating a hiqh quality, low cost land pattern for the thermal pad seems to be an open issue.
Since this new design is a prototype, we're going to use this opportunity to evaluate a recent methodolology of creating SMD (solder mask defined) windows for the thermal pad. You can read about this approach in this "Printed Circuit Design & Fab" article. The figure below is from the article and is representative of what we're trying to achieve:
Some of the goals for this methodology, which are discussed in the referenced article are:
- Utilize low-cost open through-hole via structures
- Eliminate solder wicking down thermal vias by blocking it with solder mask dams / windows.
- Ensure proper via counts to transfer heat
- Reduce stand-off variability; improving reliability
As of the date of this writing, we're in the process of finishing up our design and soliticing feedback from fabricators on the feasibility of using a low cost process for building this PCB (& stencil). We'll reflow it in house (as a starting point). Read below to review the steps we took to build the footprint / thermal pad using Altium and please post any questions or comments below. We'll update our results as the process proceeds.
Create the basic footprint
The basic footprint with thermal pad is shown in the figure below. Red is copper, and purple is the solder mask. We set the thermal pad's solder mask expansion to manual and a negative value to eliminate its definition. Remember that the solder mask is a negative image. We'll define the solder mask (windows) in the steps below
Define a single SMD Window
The upper left SMD window is defined using track and arc primitives with Altium's PCB Library Editor:
- Set the active layer to solder mask
- Draw four arcs around the upper-left four vias
- Create two tracks / lines along the upper-left exterior of the thermal pad
- Create two additional tracks to intersect with the middle via. The tracks are positioned in such a way to create a 6 mil solder mask pane line ( vertical and horizontal lines that define the window ).
- Manipulate the end points of the primitives so they intersect
- Select the primitives
- Tools -> Convert -> Create Region From Selected Primitives.
Complete the BTC Solder Mask Definition
- Copy and paste the upper left SMD Window three times to create the other windows. Use 'X' and 'Y' shortcuts as necessary to flip the windows as needed.
- Create solder mask expansions for each via hole, so they are not tented.
- Copy the SMD windows from the solder mask layer to the solder paste layer.
A look at the rendered footprint
After associating the new footprint with the device, render a 3D image of the PCB:
Note that Gerbers have been generated and have gone through a preliminary internal review. Tweaking will probably be necessary (e.g., smooting and resizing) before fabricating. We'll continue to update this article as the process moves along.