Footprint for TI DRV8811 (w/powerpad)

Here you can find discussions pertaining to finding or creating Symbols and package footprints. Anything to do with Schematic or layout parts will be placed in this discussion.

Moderator: Sunstone Moderators



Footprint for TI DRV8811 (w/powerpad)

Postby joffenb » Wed Oct 31, 2012 7:20 pm

Trying to figure out how to get around program limitations to create a footprint for the Texas Instrument DRV8811 Stepper Motor Controller.
Datasheet URL: http://www.ti.com/lit/ds/symlink/drv8811.pdf

It's basically a 28 Pin TSSOP with what TI calls a "powerpad" that requires a relatively large copper pour on top and bottom layers with 21 vias to conduct heat to the opposite side of the board.

No problems with the 28 normal pins, but creating the heat sink area with 21 thermal vias seems to be beyond the capabilities to the current program.
Any assistance would be greatly appreciated.
joffenb
 
Posts: 1
Joined: Wed Oct 31, 2012 10:21 am

Re: Footprint for TI DRV8811 (w/powerpad)

Postby Sal Hernandez » Thu Nov 01, 2012 8:06 am

The part can be created in PCB123. From the layout select Design > New Footprint to begin.

  1. Start by making sure you have the Edit Panel open. This is the large box of information you should see along the left side of you screen. If you don't see it select View > Edit Panel.

  2. Create the footprint and keep the origin at the center. Make sure you have the grid visible. In the Edit Panel click on the box next to Grid and select visible. Also, make sure that you set your units to mm in the Global View > Units section of the Edit Panel.

  3. When you create the component pads you will set you grid by pressing the g key to .325mm, 5.6mm. Then select the Add pin tool and set your pin properties in the top section of the Edit Panel.

  4. Place your pins so that they are centered around the origin, 14 pins on each side. Make sure your pin ordering is correct.

  5. Create the power pad area that will be exposed through the solder mask using a surface mount pad that is 5.18mm x 3.1 mm and drop it on the origin which should be the center of your footprint.

  6. Draw a filled polygon on the top layer over the pad. This polygon should be 9.7mm x 3.4 mm. Changing your grid to 4.8mm x 1.7mm will make this step easier.

  7. If you need this filled polygon area on the bottom layer copy the shape and paste it off to the side. Mouse over the polygon then right click and select properties. Move the polygon to the bottom layer and select OK. Move the polygon into position.

  8. Now you are ready to create the through hole vias. Change your grid to 1.3mm. Select the Add Pin tool and set the Pin properties in the top section of the edit panel. I selected Round Pin Geometry, .3556mm hole size, .762mm pad width, and checked the Tented box.

  9. Place your 21 holes on the displayed grid points.

  10. Finally you can select the Draw Polygon tool and switch to Simple Polyline in the Edit Panel to draw the body of the part and add a pin 1 reference designator. I usually change my grid to .001" and use the Draw Circle tool for the pin 1 designator.

Note: The .3556 mm hole size is only available on a multi-layer board. If you add this part to a 2 layer board the hole size will increase to .508 mm. Also, note that this part will result in drc pad to polygon errors when placed on the PCB123 layout. These errors will not prevent you from submitting an order but you should be aware that they will be reported.

I have attached the footprint that I created.
Attachments
TI.SLB
(6.39 KiB) Downloaded 345 times
Regards,

Sal Hernandez
Software Support Engineer I
Sunstone Circuits
13626 S. Freeman Road
Mulino, OR 97042
Phone: 503-829-9108 x226
Fax: 503-829-5482
User avatar
Sal Hernandez
 
Posts: 396
Joined: Wed Jul 06, 2011 12:00 am




Return to Schematic and Layout Parts (Libraries)

Who is online

Users browsing this forum: No registered users and 0 guests