Author Message
 Post subject: SO-8 Dual PowerPAK Pad questions
PostPosted: 30 May 2017, 11:37 

Joined: 06 Dec 2016, 11:12
Posts: 3
Hi - I'm trying to make the pattern for the SO-8 Dual PowerPAK for a dual FET chip (Si7942DP). The Drain connections of the chip use two numbered pads (7&8 and 5&6) and then has a plane that goes underneath the chip and connects the pads. See the attached link to the picture. I tried to do this by using normal pad layout and numbering and then drawing a filled rectangle to connect the pads. While it looks fine in the pattern editor, when I go to layout and attach a filled plane, it will not connect to the filled rectangle portion properly. Can anyone recommend how to go about properly creating this type of pad?

Picture of pattern:

Picture of layout showing how filled plane behaves:

Thanks in advance!
- Dennis

 Post subject: Re: SO-8 Dual PowerPAK Pad questions
PostPosted: 30 May 2017, 16:15 

Joined: 20 Jun 2015, 14:39
Posts: 934
Create an SO-8 pattern with only 6 pads (refer to illustrations below)...
1) Create the pattern in the 2D CAD program of your choosing and substitute pads 5 & 6 with one pad that takes the shape of the combined pad 5 + pad 6 + its overlapping plane + a poorly-documented vertical pin/tab.
2) Do the same for pad 7 + pad 8 + its overlapping plane + another poorly-documented vertical pin/tab.
3) Export as a DXF file, then import the DXF file into the Pattern Editor. (Same DXF Units, Import Mode: Add, Convert to: Top Signal, [X]Fill Closed Areas)
4) Right click on each filled object and select Convert to Pad in the pop-up menu.
5) Re-number the combined 5+6+plane+vertical-pin/tab pad to "D2".
6) Re-number the combined 7+8+plane+vertical-pin/tab pad to "D1".
7) Resave the pattern.
8) Create a 2-part 6-pin component in the Component Editor with the same pin numbers.
9) Attach the new pattern to it and resave the component.
Now when you use the new SO-8 "6-pin" pattern, it will come with all the right copper shapes. Take note that the special pads will want to connect to traces near their centers, so you may have to change the grid to a smaller size if you want to route a trace out one of old pad locations (formerly pads 5, 6, 7 & 8) to make it appear more "conventional". Also take note that copper pours may interact with the new pattern in an unexpected manner when you need to connect to the special pads using thermal spokes. It shouldn't result in anything outrageous, though, and you can always select a different thermal spoke pattern/orientation. At least you won't have to deal with creating tiny planes for the pattern in the PCB Layout editor.

I have attached a copy of the special SO-8D pattern library, component library and 3D model (STEP file), along with ASCII versions of those library files if you are using an older version of DipTrace. Everything is contained in the zip folder named "" below. After importing, you will have to link the 3D model to the pattern and then attach the pattern to the component since I don't know how your directories are set up.

Please double-check all dimensions and pinouts against the manufacturer's datasheet. I have never used this component so I cannot guarantee a proper fit or fire resistance.

You do not have the required permissions to view the files attached to this post.


Display posts from previous:  Sort by  
Post new topic Reply to topic  [ 2 posts ] 

All times are UTC - 5 hours [ DST ]

Who is online

Users browsing this forum: No registered users and 7 guests

You cannot post new topics in this forum
You cannot reply to topics in this forum
You cannot edit your posts in this forum
You cannot delete your posts in this forum
You cannot post attachments in this forum

Search for:
Jump to:  
Powered by phpBB © 2000, 2002, 2005, 2007 phpBB Group