Mind Chasers Inc.
Mind Chasers Inc.

Build a BTC Footprint with Thermal Pad using SMD Window Approach and Altium Designer

BTC packages with thermal pads present a myriad of challenges. A recent approach to BTC PCB land pattern design is the use of an SMD Window. This article shows the construction of such a land pattern and results after reflow.



BTC's (Bottom Termination Components) are everywhere. These are the devices with terminations / leads hidden under the package and often have large thermal / ground pads in the center. We use them extensively on all new designs and are continually seeking to develop the best process possible to produce low cost, reliable, high quality solder joints with a low percentage of voiding.

This article reviews a subset of our process and results with Texas Instrument's DP83867CS Gigabit Ethernet PHY device. This device is packaged in a 7 mm2 48-pin QFN package with a 4.1 mm2 thermal pad. For this type of package, we have adopted a methodolology of creating SMD (solder mask defined) windows for the thermal pad. Our in-house CAE tool is Altium Designer, and we build our BTC footprint using their IPC Footprint Wizard followed by manual customizations for the thermal pad and some additional fine tuning of the footprint features. We find that we can quickly build customized BTC footprints in a matter of minutes using this process.

You can read about the SMD Window approach in this "Printed Circuit Design & Fab" article, and the figure below is from the article and is representative of what we're trying to achieve:

Figure 1. Example SMD Window footprint
SMD Window Example

*Source: M.Kelly, M.Jeanson et al, IBM Corporation

Our goals for this methodology, which are discussed in the aforementioned article, include:

  • Utilize low-cost, open, through-hole vias
  • Eliminate solder wicking down the thermal pad vias by blocking it with solder mask windows.
  • Use sufficient number of vias to transfer heat from the thermal pad
  • Reduce stand-off variability and improve reliability

Create the basic footprint

The basic footprint with a single, monolithic thermal pad is shown in the figure below. Red is copper, and purple is solder mask. In Altium, 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

Figure 2. Basic BTC/QFN Footprint
Basic Footprint

Note that some manufacturers still recommend this basic footprint for their BTCs / QFN packages. We consider this a quick and dirty approach. The primary disadvantage with this approach is that solder can run down the via holes during reflow, create shorts on the wiring side, and also impact the quality of the connection to the thermal pad.

Define a single SMD Window

The upper left SMD window is drawn first using a single polygon region. Before placing the polygon, we perform all the geometry calculations. We strive to keep board cost to a minimum, but we also choose a PCB fabricator that can deliver things like high quality 8 mil drill holes and 6 mil solder mask webbing.

Figure 3. Polygon defines the shape of single SMD window
Primitives define shape of SMD window

Complete the Thermal Pad Solder Mask Definition

  1. 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. Make sure the grid enables positioning each window with perfect symmetry
  2. Manually set the solder mask for each via, so they are not tented.
  3. Copy the new SMD window solder paste polygons and paste them on the solder paste layer. Note that you may wish to reduce your solder paste openings.
Figure 4. Completed BTC thermal pad
Completed BTC thermal pad

A look at the rendered footprint

After associating the new footprint with the device, the rendered 3D image of the PCB is shown below:

Figure 5. 3D rendered image of land pattern on PCB
3D rendering of footprint on PCB

X-ray the board

The figure below shows an X-ray image that we took of our device and footprint after the board was run using our in-house quick-turn process. Note that we utilize vapor phase batch ovens for reflow, and the X-ray image utilized 80kV power. We're encouraged by the results, but also working to improve the process.

Figure 6. X-ray image of BTC device on PCB
X-ray image of BTC

Didn't find an answer to your question? Post your issue below or in our new FORUM, and we'll try our best to help you find a solution.

And please note that we update our site daily with new content related to our open source approach to network security and system design. If you would like to be notified about these changes, then please follow us on Twitter and join our mailing list.

Related articles on this site:

mailing list:

Date: Nov. 11, 2017

Author: Chandru


Small child card after reflow process getting one corner liftup , what is the exact issue

Date: Nov. 11, 2017

Author: Mind Chasers


Hi Chandru, Some things to look at: too much solder paste deposited on the thermal pad, warped PCB, or non-uniform pads & stencil apertures causing the package to lift or dip on one side / corner. What type of package are you using? Are the land pattern pads uniform around the device?

Add a new comment here or reply to one above:

For enhanced features and capabilities, please sign in or authenticate using a popular third party

your email address will be kept private

to upload an image

previous month
next month