0
\$\begingroup\$

Looking at TI's TPS56339 and looking at what TI outputs for Altium opens up some questions for me.

In the following image, the highlighted component is the TPS56339. enter image description here

  1. Has the assembly process improved such that thermal relief is not necessary or for this type of PCB must you go with specific assembly houses that can bring the board up evenly ? In a general sense, for a SMPS, should thermal relief be added to pads ?

  2. What is the possible reason for the large quantity of vias here ?

The image below is a zoomed into the converter where we can see the copper and silkscreen and soldermask. enter image description here

  1. Pin 1 (top left of the image) is riddled with vias. From an assembly point of view, would this be a problem (solder theiving or other) ?

  2. What overall recommendations would you have to improve assembly without hindering the performance of the switcher too much ("too much" is whatever you think).

\$\endgroup\$
  • \$\begingroup\$ How did you get the Altium version of the design? Is it possible the design was initially made with another tool and a solder mask tenting specification was lost in translating it to Altium? \$\endgroup\$ – The Photon Apr 13 at 16:08
  • \$\begingroup\$ @ThePhoton TI Webbench which supports a variety of formats, so its quite possible that certain information was lost between cad tools. \$\endgroup\$ – efox29 Apr 13 at 16:11
1
\$\begingroup\$

Has the assembly process improved such that thermal relief is not necessary or for this type of PCB must you go with specific assembly houses that can bring the board up evenly?

It is possible to assemble this type of design.

It is probably worth checking with your assembly shop to be sure it falls within their recomendations (and compare between shops if necessary).

What is the possible reason for the large quantity of vias here ?

They provide a thermal path to heat-sink the IC.

Pin 1 (top left of the image) is riddled with vias. From an assembly point of view, would this be a problem (solder theiving or other) ?

I agree this is a possible problem. Solder is likely to wick into the vias, starving the joint to the IC pin.

What overall recommendations would you have to improve assembly without hindering the performance of the switcher too much ("too much" is whatever you think).

Either move the vias (slightly) further away from the pad and tent them on the top side, or have the vias filled before assembly (with some cost impact).

If you don't need to operate this regulator near its thermal limits, then you could consider thermal relief for the two ground pads (as well as for the left pad of the inductor).

Edit

Looking at the photo of the actual board in TI's datasheet for the evaluation board, there are no solder mask openings at the locations in question:

enter image description here

Most likely, the board was designed with filled and tented vias (or possibly just tented vias), but the requirement to tent the vias was lost in translating the design from some other tool to Altium.

| improve this answer | |
\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.