How to make global fiducials in Allegro
Fiducial reference points are necessary in a circuit board if you are going to assemble your PCB using automated pick and place machines. Automated assembly machines require incredible precision to accurately place a 0201 size resistor or a 2mm x 2mm chip-scale micro BGA.
A fiducial is the reference point on the PCB for assembly machines. It helps the machine to recognize your board orientation and direction. Fiducials can be placed on the top copper layer; they are not placed on the mask or silk layers, because they are not as precisely aligned to the parts as the copper layer itself.
There are global and local fiducials. Global fiducials are used to locate the position of all of the land patterns on a PCB. A local fiducial is used to locate the position of an individual land pattern on a PCB.
Below you’ll see the steps needed to make global fiducials in Allegro, where we use two fiducials on either corner of the PCB. The farther away they are, the better the precision.
Fiducials can have many different shapes: they can be circular, square, triangular, diamond-shaped, and so on. Most commonly, they are circular, and their typical size is 1.0 mm (dia) for the copper pad with a 2.0 mm (dia) stop mask. A keepout of 3.2mm dia is needed around the fiducial to avoid having planes or traces under the fiducials.
Steps to making global fiducials in Allegro 16.6:
Step 1. Create SMD Padstack for a 1mm circular pad/2mm Solder mask.
Step 2. Open Allegro PCB Librarian XL, then go to File and click on New. Enter the Drawing Name, after that click on Drawing Type, select Mechanical symbol and finally click OK.
Step 3. Go to Layout, then go to Pins. Select Padstack and then place the padstack at the origin (0,0). After that, right-click and then click on Done.
Step 4. Go to Shape, then select Circular. After that, set Class/Subclass as Package Keepout/Top, and then select Place circle at the options tab. Set Radius as 1.6mm and place the circle at the origin (0,0).
Step 5. Repeat step 4 with Class/Subclass as Route Keepout/Top
Step 6. Save the design
Step 7. Open Allegro PCB Design, then click on Place, after that select Manually, then go to the Advanced Settings tab. Pick Library and go to the Placement List tab. There you need to scroll down and select Mechanical symbols to pick the symbol that you have created. After that, place it into the PCB layout. Finally, right-click and then click on Done.