JEDEC MO-240 AA ?

HI, for the JEDEC MO-240 Var AA for a Fairchild FDMS7650 etc.

This is like an SO8 with a big heat pad inthe middle where it is connected to 4 of the outer pads.
In this part it has 4 common pads for the "Drain".


If the component layout for this has the big centre pad and the 4 drain pads all within the same sodler resist clearance, so that there is no sodler resist between the 4 drain pads and the heat slug - when reflow soldering would there be a tendency for the solder from the 4 pads to wick back onto the heat slug leaving them with poor connection?

The manufacturers recommended footprint is:


Now given that they are bonded to the same heat slug on the component I'm not sure it really matters.
In the past I usually make this with a big rectangular pad for the slug with its own solder resist and 4 separate pads for the drain connections. This gives each one their own solder resist shape & hence a gap between the 4 & the slug.

So I am wondering whatIPC7351 says about it? what others would do about the above and where to start in the wizard for this - what SMT family to choose to start etc?

Cheers,
Matthew

IPC does not have any guidance on non-standard component packages.

You should use the mfr. recommended pattern. This is a very easy part to create in FP Designer.

In the Sample FPX that comes with Library Expert, look at these footprints -

1. FAIRCHILD_FDMC8878

2. IRF_IRFHM4226TRPBF

3. FAIRCHILD_FDMS86150

4. VISHAY_SI7115DN

Nick will help you with your license issue.

The past mask of the Thermal Pad should not touch the paste mask of the smaller pads.

We can relocate the Thermal Pad Paste Mask internally and then output a XML FPX file that can be opened in Library Expert. Do not co-minge XML FPX with ASCII FPX as they are 2 different formats.

I would highly recommend to use Parts on Demand and Request a Part - www.pcblibraries.com/pod

Here is a XML FPX sample of the Thermal Pad Paste Mask moved away from the smaller pads -

Sample_Thermal_Pad_Paste_Mask_XML_FPX.zip

The Solder Mask is removed from all metal surfaces.

Full Paste Mask coverage is applied to the Lead Terminals and 50% reduction on the Thermal Pad.

There doesn't seem to be any guidance from the component mfr. (CM) on this subject of "Solder Dam" that would prevent the Lead Terminal solder from wandering onto the Thermal Pad during reflow. I would think that the Solder Mask would have a break line to prevent that. The CM's should have better drawings and illustrations.

I'll bring this subject up at the next IPC-7351 executive committee meeting at IPC APEX on Wednesday February 25. But I need to gather information from the industry and assembly shops to present it to the committee.