«

»

Jan 11

Orcad 16.5 Custom Footprint

Continuing from the padstack design for the FDN340P this post focuses on the footprint layout.  One word of caution, I’m just learning how to create these footprints so it’s likely that there are problems with the footprint.  I’m not sure if the silkscreen overlap will be a problem, however I plan on figuring that out sometime down the road.

 

Start Orcad PCB Editor. Create a new package with File->New->Package.  Set the name and directory as appropriate.

 

Change the color of the origin marker and move the origin to the middle of the screen.

Color Options->Drawing Format. Change Drawing_Origin to white.

Setup-> Change Drawing Origin

Set the User Units to millimeters since this is the demension provided in the drawing.

Setup->Design Parameters->Design->User Units

 

Now that the workspace is setup it is time to begin placing pins.  Assuming the directories have been set up properly you should be able to select the previoulsy generated padstack in the options menu to the right (FDN340P).

Layout-> Pins

Options -> Select Padstack.

 

The easiest method for placing pins is going to be the command window at the bottom of the screen.  Some math will be required, but if you can remember how to add and subtract you’ll be fine.  In my case I want to keep the center of the Mosfet body alligned with the origin.  From the datasheet the pads will end up at the locations used in the commands below.

1
2
3
x -0.95 -1.1
x 0.95 -1.1
x 0 1.1

Right Click -> Done to complete pad placement and click “Add Rect” to draw the body outline.

1
2
x -1.46 -0.7
x 1.46 0.7

Next we’ll draw lines for the silkscreen.  I’m unsure whether the method I take here will cause problems further down the road, but I’m going to go for it and see what happens.

Use Add->Line and set the parameters on the options to the right.  Make sure “Silkscreen Top” is selected and set the thickness to 0.2.  Setting line lock to 90 isn’t entirely necessary but can be helpful if you’re drawing the lines manually.

 

1
2
3
4
5
x -1.46 -0.7

iy  1.4

ix 0.96
1
2
3
4
5
x 0.5 0.7

ix 0.96

iy -1.4
1
2
3
x -0.45 -7

x  0.45 -7

In order to easily place a circle indicating pin 1 the grid size should be reduced to 0.1mm spacing.  Manually place the circle near pin 1 on the workspace.

Setup->Define Grid

Add->Circle

After placing the pin 1 indicator we will place a top bound rectangle to model the hight of the component.  Click “Add Rect” and change the rectangle options to “Package Geometry” and “Place Bound Top.”  Set the coordinates to the same values used to place the initial body rectangle.

 

1
2
3
x -1.46 -0.7

x 1.46 0.7

Set the package high through Setup->Areas->Package Heights.  Click on the package boundary and set the height in the options menu to the right.  The datasheet indicates a maximum height of 1.12 mm.

 

To complete the footprint a set of reference designators need to be defined.  Do this through Layout->Labels->Refdes.  Place an “Assembly Top” on the body of the Mosfet.  Enter “Q?” as the value.  Place another RefDes this time as a “Silkscreen Top” above the Mosfet footprint. Finally, save the footprint and the design is complete.


Sources:

Footprint

Datasheet

 

 

Leave a Reply

Your email address will not be published. Required fields are marked *

You may use these HTML tags and attributes: <a href="" title=""> <abbr title=""> <acronym title=""> <b> <blockquote cite=""> <cite> <code> <del datetime=""> <em> <i> <q cite=""> <strike> <strong>