[PCB_FORUM] Re: About Thermal Pad Land pattern

Luo,

I forgot to say don't put SOLDERMASK window pains on the thermal pad.

Also, in figure 9 of the TI app note, TI states "Cross hatching - Recommended", 
This figure assumes that the vias are open and not filled with via filler.

Open vias reduce the solder volume under the Thermal Pad by allowing solder to 
run out the vias toward the secondary side.

Best of luck,

Dave


Dave Seymour
Ixia
919.267.4840
________________________________
From: Dave Seymour
Sent: Wednesday, July 01, 2009 10:15 AM
To: 'icu-pcb-forum@xxxxxxxxxxxxx'
Cc: 'Luo.Yu-Ming@xxxxxxxxxxxxxxxx'
Subject: RE: About Thermal Pad Land pattern

Luo,

We make our thermal pads the same size as the IC.

However, IF the vias are plugged with non-conductive via filler, THEN we will 
"Window Pain" the Solder PASTE mask to deposit less paste for reflow.

I attached a TI app note and if that doesn't come through the link is below.

http://focus.ti.com/general/docs/lit/getliterature.tsp?literatureNumber=sloa120&fileType=pdf

After reading the above, the assembly process list may make more sense.

1)       Secondary Paste is applied
2)       Secondary Parts placed
3)       Secondary side reflow ( if the Thermal Pad is on the back, this will 
cause problems on the primary side because of solder flowing through to the top 
side)


4)       Primary pasted is applied
5)       Primary parts placed.
6)       Primary side reflow  ( if the Thermal Pad  is on the primary side, the 
solder will flow to the back side but not interfere with the paste process on 
secondary side)

Now, one could argue that the Thermal Pad on the primary side will be starved 
for solder, but I don't believe that we have experienced this situation, or 
maybe just has not looked.

Which lead to the next thing, which is paste volume on a Thermal Pad.

If the Thermal Pad vias are filled with Peter's paste and the entire Thermal 
Pad is open to paste, then volume of paste on the Thermal Pad will tend to lift 
the part up off the land pattern during reflow.

I've had parts on designs completely float off of the Land pattern during 
reflow on the dome of solder paste.

And the solution to this is window pains in the stencil.

Now for a different point of point view

The attached is a guide from TI which states that secondary solder protrusions 
are ok and the Thermal Pad won't be starved for solder.
But, that is conditional upon the boards being X-rayed and verifying that 50%, 
according to TI, of the Thermal Pad is soldered.
AND TI did not state the condition where the Thermal Pad is on the back side of 
the design with the solder protrusions interfering with the top side paste 
process.


Hope this helps.



Dave Seymour
Ixia
919.267.4840
________________________________
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx 
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of 
Luo.Yu-Ming@xxxxxxxxxxxxxxxx
Sent: Wednesday, July 01, 2009 4:49 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] About Thermal Pad Land pattern

Hi, All,

Usually, we design thermal pad land pattern as same size as the chip thermal 
pad. Now our SMT engineer suggest separating the  thermal pad to several little 
rectangle area with soldmask on board, to increase joint area. Are you doing 
like this? What is the benefit and risk? where can I get any article for 
reference?

Thanks a lot. Any input would be great appreciate.

Best Regards,
Luo.

Other related posts: