The concern I have is the pad is calculated at 0.32 mm and if we get a batch of parts that are created at the max tolerance the pin will overhang the pad on the b measurement.  

Is this correct or am I missing something?  

What do I tell my Engineers?

What is the component family of the footprint you're creating?

I had my librarian re-create it with a newer version of library expert with the same results.

If this is troubling you and your engineers then do this. 

Go to "Tools > Options > Terminals > Surface Mount > Flat No-Lead (Side) > Side goal" and change the value from -0.04 to -0.02 and your pad width will recalculate to 0.36 mm

All the values in Footprint Expert are editable. If you don't like a value set forth in the IPC-7351B standard then change it. 

Here is the Flat No-Lead Table 3-15 in IPC-7351B (and an explanation of the negative solder joint goals: 

 

We have an IPC library and are contently questioned on parts created for one reason or another.  

If it does violate IPC suggestions I will be creating this as alternate part.

IPC-7352 is NOT a Standard. It's a Generic Guideline for Land Pattern Design. 

There's no such thing as violating a Guideline. A Guideline is a suggestion or recommendation. 

You mentioned that the default side solder joint goal for a Flat No-Lead QFN is 0.03 mm smaller than the maximum terminal lead width. 

Tell your engineers that you're adjusting the "Guideline" by less than 1 mil because you're paranoid that the pad width is too small. 

The main reason why the Guideline suggests a -0.04 mm side goal is because of the 0.40 mm pin pitch QFN where the pad sides would be too close together and violate your minimum pad to pad spacing. 

Also, you can't run a trace between a 0.50 mm pin pitch QFN. So the maximum lead hanging over the pad slightly won't affect anything. 

Which values are you using for fabrication/assembly tolerances in this case? 

The default values? 0.00 mm? 

Regards.

David

But all the negative solder joint goals are 0.00 too. 

There is an IPC-7352.opt file that updates all the options to do this. 

However, if you open the IPC-7352.opt file, don't forget to save it under a different name before you start editing it because it will be overwritten with a new installation.