TPS22921 solder requirements

Michael,

I will redirect to our QA/Processing team and have them post here.

Regards,

Wade

Michael,
I am moving this to the correct forum for support.
Regards,
Wade

Hi Michael,

I will talk with one of our packaging experts and get back to you soon.

Thanks,

Alek Kaknevicius

Hi Michael,

I have a few questions regarding your issue:

1. Is this position error due to placement or does it happen during reflow?
2. Would you be able to send us any pictures or x-rays of the problem so we can see exactly what is going on?  Any GERBER files of the PCB layout you might have would also be helpful.

Thanks,

Alek Kaknevicius

Hello Alek

Issue with soldering of the BGA was brought to light with a recent failure of the TPS22921 part.  In the analysis it was observed that two of the 6 pins showed power solder joints.  I am looking to see if there are any specific requirements on how this part should be soldered to a board base on its physical size and the 6 BGA.  My theory is that when placed on a board prep to solder, the solder paste may not be even and the melting of the solder past my not be event.  This results in the part tilting as the solder melts resulting in one or more pins not obtaining good solder joints due to a change in gap distance.

Pictures:  AttachedPoor solder joints.docx

 

 

Hi Michael,

Thank you for the x-rays and pictures, the issue is much clearer now.

Based on the x-ray, it seems as though the metal between all 6 bumps is uneven.  What I mean is that there are larger traces on bumps A1 and C1, and this will cause the package to tilt away from the "2" side and towards the "1" side during soldering, creating opens on the "2" side. 

The below picture on the right shows the proper way to bring traces to this type of package.  The traces connecting to the bumps should be no thicker than the bump diameter itself.  This places the same amount of metal on each pad and balances the way the solder spreads during reflow.

In general, it is best to follow these guidelines:

• Only one connection per bump (no bump-to-bump connections).
• The traces to each bump should be the same thickness.
• When possible, all traces leave the package in the same (outwards) direction.

For further analysis of your specific issue, we would need the following information:

1. PCB layout. Soldering pad size, solder mask opening. (gerber file preferred)
2. Stencil aperture and thickness
3. Reflow profile
4. Pick and place machine type and nozzle size.

Regards,

Alek Kaknevicius

Michael,

To expand on what Alek just wrote, on the illustrations above, the traces need to be no wider than the recommended pad diameter until they clear the soldermask ring (plus allowance for soldermask registration) and then can be widened to any desired width or connected to a plane.

An alternative is to use soldermask defined pads, where the metal is larger than the soldermask openings for all pads and the soldermask opening diameter (namely 0.225 - 0.23mm) defines the soldering pad. Metal pads should be made larger than the soldermask opening to allow for soldermask mis-registration. This approach makes all pads exposed to soldering the same size regardless as to how you connect your traces to the pads.

Hello Alek

It has been several months since I last talked about this issue, and we did have the board manufacture make some adjustments to the solder reflow temperature profile and stencil aperture.  We are still having some problems but is has been reduced.   I want to capture the info you requested in a previous conversation and send them.  do I use this form and send as an attachment?

Michael Mancuso

Reliability Engineer

Varian Medical Systems

Hi Michael,

I am a bit confused about what you are asking.  Are you looking for additional information, or do you want to consolidate the information in this thread to send to the manufacturer?

Thanks,

Alek Kaknevicius

hello Alek
On Feb 19 2015 you stated that additional info is required for further analysis by a TI application eng. I would like to send the specific documents to a TI application eng to evaluate our design regarding the implementation of the TPS 22921 device. Who do contact and I send the material :

1.PCB layout. Soldering pad size, solder mask opening. (gerber file preferred)
2.Stencil aperture and thickness
3.Reflow profile
4.Pick and place machine type and nozzle size.

I do not want to put the info on this form
Mike Mancuso

Hi Mike,

Thank you for the clarification.  You can send this information to me (a-kaknevicius@ti.com) and Ernesto Rey (Ernesto.Rey@ti.com).

Thanks,

Alek Kaknevicius