Creating Footprint in Allegro PCB Design
Table : Allegro PCB Design Tutorial
Creating Footprint or Symbol in Allegro
Footprints or symbols are the electrical plus mechanical description of the component. It is created from the datasheet of the components. For this tutorial we will be creating the symbols for the 0603 resistor and the two pin Header.
Click on Start -> Allegro SBP 15.2 -> PCB Editor -> Select Allegro PCB Design 610 ( PCB Design Expert) -> Click OK.This will open up the Allegro software. Click on File -> New. In the “Drawing Type” Select Package Symbol. In the drawing name write R0603_1. Also browse to directory C:/learnallegro/symbols/. We will save this symbol in directory C:/learnallegro/symbols/.
Before we start creating Symbols, we will have to do some preparation. First, Click on Setup, Drawing Size. In the dwawing extents – make left X and lower Y to, say -1000, -1000. Also reduce the width and height to some resonable value, say, 10000 and 8000 respectively.
Next, Allegro should have some way to know, if it can use the padstack we created in the last page. Do do this- Click on Setup -> User Preferences -> -> In Categories, select Design Paths.click on the triple dotted rectangle in front of padpath.Click on New ( Insert) Button. Point to the directory where you have saved your own created padstack. Click Apply and comeback to main Window. Click on Tools -> Padstack -> Refresh Padstack. Click Refresh.
We will now add the two pads at coordinates (-31,0) and (31,0).Clcik on Layout -> Pins. In the options tab, click on the rectangle in front of Padstack. From the list that follows, select the padstack named SMD30_38. Click ok. Now go to command window and write x -31 0. Right click and click done. You you happen to place it at some other place, you can change it by Edit move. You may also like to setup approprite grid by using Setup -> Grids.
Do the same thing for the second pin and place another SMD30_38 padstack at (31,0). This completes the pins placements. We will next add a rectangle around it, which will be used in silkscreen. Click on Add -> Rectangle. In the Options Tab -> Select Package Geometry under Class and Silkscreen_Top in the Subclass. Now come to Command> window and write x -70 -35. This is the left bottom coordinate of the rectangle. Next write x 70 35 in the Command>. This will create a silkscreen rectangle around the padstack. We will next add a placebound rectangle, which will be used in detecting any error if anything is placed too close to this component. Click on Add -> Rectangle. In the Options Tab -> Select Package Geometry under Class and Place_Bound_Top in the Subclass. Now come to Command> window and write x -70 -35. This is the left bottom coordinate of the rectangle. Next write x 70 35 in the Command>. This will create a Place Bound rectangle around the resistor.
We will now add reference designation, that will be required with printing silkscreen and for manufacturing. Click on Layout -> Labels -> RefDes -> Choose the class as Ref Des and Sub Class -> SilkScreen_Top. Click somewhere to the right of the resistor and write R?. This will create a placeholder for printing silkscreen. We need another label for Manufacturing. Click on Layout -> Labels -> RefDes -> Choose the class as Ref Des and Sub Class ->Assembly Top. Click somewhere to the top of the resistor and write R?. This will create a placeholder for Assembly. Save the file as R0603_1.dra in the directory C:/learnallegro/symbols/.
This completes Creation of the Symbol name R0603_1.
We will similarly create another symbol HEADER2 that will use the through hole padstack. The procedure is similar to above. Just use the through hole padstack named Pad50cir35d , and place them at coordinates (-50,0) and (50,0).
Following are the links to some video Flashes that will help you understand Padstack creation.