My company has finally installed PCB Footprint Expert on our computers. Time to update the old .xml preference file to the new .opt file !

By default, the IPC-7351C.opt file uses a Thermal Tab Paste Mask Percentage of 50%.

The IPC-7351B states that "The default paste mask for these pads is 40% of the overall land area".

May I ask why this 10% difference ? I know things have changed since the realase of IPC-7351B. 

Is it just a guess or is there some document that talks about this 50% amount ? 

EDIT : I just read PCB FOOTPRINT EXPERT documentation more closely and found this line : "IPC- 7093A figure 3-10 recommends that the stencil design provide 50 – 60% solder paste coverage on the thermal pad area."

Follow up question : why the difference between IPC-7351 and IPC-7093 ?

Another topic : What do you think about vias in thermal tabs ? Depending on the person I ask this question, I get two main answers : 

And this article, linked in the previous post :  https://pcdandf.com/pcdesign/index.php/magazine/10676-btc-design-1603" rel="nofollow - https://pcdandf.com/pcdesign/index.php/magazine/10676-btc-design-1603

It includes through-hole and should be released next month. 

There is an IPC-7352 .opt file in the main folder. 

For thermal tabs, there is a new Option to Solder Mask Define the pad. 

This dams in the paste mask and prevents it from flowing. 

See this article:  https://www.pcblibraries.com/forum/ipc7093a-btc-qfn-solder-mask-defined-thermal-pad_topic2154.html" rel="nofollow - https://www.pcblibraries.com/forum/ipc7093a-btc-qfn-solder-mask-defined-thermal-pad_topic2154.html

Maybe I am missing something, but the option for solder mask define is not easily usable in QFN with tab. Yes you can set a paste mask pourcentage. The SM pattern will match 1:1 with the solder paste pattern. But the option for minimum pattern space is non functional.

Hence the software will arbitrarily decide how many little square it will generate to meet the required paste %. But without the minimum pattern space options, there is no way to guaranty that the via holes will be covered with solder mask. The only indirect way to control the pattern spacing is to reduce the paste %, which is not ideal.

Best regards,

They did extensive testing and have all the results published. 

Solder Mask defined Thermal Pad technology eliminates Thermal Pad Paste Mask voids and allows vias to be unplugged, which saves 10% on fabrication costs. 

They also published thermal relief percentage for every via hole and calculated 9 via holes is the most the thermal pad requires. Any additional holes are have minimal thermal reduction. 

Also, the paste mask aperture openings on thermal pads contour around the vias adding extra paste mask percentage. 

I know that Footprint Expert can't do this right now, but it's future technology.