Pad Making--Allegro Tutorial

Use Pad Designer to make pads
The job of making pads in Allegro is called Pad Designer, and all SMD pads, through-hole pads, and vias are made with this tool.
Open the program->Cadence SPB 16.2->PCB Editor utilities->Pad Designer, and the pad-making interface will pop up, as shown in Figure 1.1.

Select the unit in the Units drop-down box. Commonly used are Mils (millimeters) and Millimeter (millimeters). Choose according to the actual situation.
Select the type of drilling in the Hole type drop-down box. There are three options:

• Circle Drill: circular drilling;
• Oval Slot: oval hole;
• Rectangle Slot: rectangular hole.

Select the metallization type of the hole in the Plating drop-down box. There are two commonly used ones:

• Plated: metalized;
• Non-Plated: Non-metalized

Generally, the pin pads of through-hole components should be metalized, while the component mounting holes or positioning holes should be non-metalized.
Enter the drill diameter in the Drill diameter edit box. If you choose an ellipse or a rectangular hole, the two parameters Slot size X and Slot size Y correspond to the X and Y-axis radius of the ellipse and the length and width of the rectangle respectively. In general, it is enough to set the above parameters, and other parameters can be set by default. After setting, click the Layers tab to enter the interface as shown in Figure 1.2.

If you are making the pads of surface mount components, tick the Singel layer mode check box. Parameters to be filled in:

• Regular Pad on the BEGINLAYER layer;
• Regular Pad on the SOLDEMASK_TOP layer;
• Regular Pad on the PASTEMASK_TOP layer.

As shown in Figure 1.3.

If it is a through-hole pad, the parameters that need to be filled are:

• Regular Pad, Thermal Relief, Anti Pad on BEGINLAYER layer;
• Regular Pad, Thermal Relief, Anti Pad on the DEFAULTINTERNAL layer;
• Regular Pad, Thermal Relief, Anti Pad on the END LAYER layer;
• Regular Pad on the SOLDEMASK_TOP layer;
• Regular Pad on the PASTEMASK_TOP layer.

As shown in Figure 1.4.

The Thermal Relief in the three levels of BEGINLAYER, DEFAULTINTERNAL, and ENDLAYER can choose the default connection methods provided by the system, namely Circle, Square, Oblong, Rectangle, and Octagon. In the PCB, these connection methods are simple '+' shapes. Or'X' shape. You can also choose your own hot air pad connection method, that is, choose Flash. This requires a Flash file to be prepared in advance (see Section 2). See the following introduction for the setting of these parameters.

  PCB QUOTE  

Knowledge in PCB Pad

The following introduces some knowledge in a pad.
A physical pad contains three pads, namely:
Regular Pad: Regular pad, the pad seen in the positive film is also the basic pad of the through-hole pad.
Thermal Relief: Hot air pad, also called a flower pad, is effective in the negative film. It is used to connect the pad and copper in the negative film.

• Anti Pad: An isolation pad, also effective in the negative film, is used to isolate the pad and copper in the negative film.

• SOLDEMASK: Solder mask, where the copper skin is exposed and needs to be soldered.

• PASTEMASK: The size of the steel mesh window.

Selection of land name level size of surface mount component package

Selection of land name level size of surface mount component package:

• 1. BEGINLAYER
• Regular Pad: Determined according to the pad size provided in the device data sheet or the device pin size measured by itself.
• Thermal Relief: Usually 20mil larger than Regular Pad. If the size of Regular Pad is smaller than 40mil, reduce it appropriately as needed.
• Anti Pad: Usually 20mil larger than Regular Pad. If the size of Regular Pad is smaller than 40mil, reduce it appropriately as needed.
• 2. SOLDEMASK: Usually 4mil (0.1mm) larger than Regular Pad.
• 3. PASTEMASK: Same as SOLDEMASK. Selection of the dimensions of each level of the in-line component package pad:
• a. BEGINLAYER
• Regular Pad: Determined according to the pad size provided in the device data sheet or the device pin size measured by itself.
• Thermal Relief: Usually 20mil larger than Regular Pad.
• Anti Pad: Same as Thermal Relief setting.
• b. ENDLAYER

Same as BEGINLAYER layer setting.

• c. DEFAULTINTERNAL

The parameters of this layer are set as follows:

DRILL_SIZE >= actual pin size + 10MIL
Regular Pad >= DRILL_SIZE + 16MIL (0.4mm) (DRILL_SIZE<50)
Regular Pad >= DRILL_SIZE + 30MIL (0.76mm) (DRILL_SIZE>=50)
Regular Pad >= DRILL_SIZE + 40MIL (1mm) (when the drilling is rectangular or oval)
Thermal Pad = TRaXbXc-d where TRaXbXc-d is the name of Flash (described later)
Anti Pad = DRILL_SIZE + 30MIL (0.76mm)
SOLDERMASK = Regular_Pad + 6MIL (0.15mm)
Flash Name: TRaXbXc-d

in:
a. Inner Diameter: Drill Size + 16MIL
b. Outer Diameter: Drill Size + 30MIL
c. Wed Open: 12 (when DRILL_SIZE = 10MIL or less)
15 (when DRILL_SIZE = 11~40MIL)
20 (when DRILL_SIZE = 41~70MIL)
30 (when DRILL_SIZE = 71~170 MIL)
40 (when DRILL_SIZE = 171 MIL or more)
Ensure that the width of the joint is not less than 10mil.
d.Angle:45

When making the pad, it must be noted that the size of the Anti Pad must be larger than the Regular Pad, otherwise, the copper-clad layer will cause a short circuit. Because allegro's file management is a bit mixed, each pad will be saved in a file, so when naming the pads, try to show the shape and size of the pads, so that it can be easily managed and reused in the future.

Making around hot air pad

Open Program->Cadence SPB 16.2->PCB Editor, select File->New, as shown in Figure 1.6.

The New Drawing dialog box pops up, as shown in Figure 1.7.

Enter the file name f55cir40_15 in the Drawing Name edit box, the suffix name is automatically generated. Select Flash symbol in the DrawingType list box, and click OK.
Click Setup->Design Paramenters to open the design parameter setting dialog box, and click the Design tab, as shown in Figure 1.8.

Select the unit Mils in User Units. In Accuracy, set the number of decimal places. The default is two digits. Enter 200 for Width and 200 for Height to set the size of the drawing area. You can adjust the size appropriately according to the pad you made, then enter -100 for Left X and -100 for Lower Y to set the coordinates of the lower-left corner of the drawing area, So that the origin coordinate (0, 0) is at the center of the drawing area, otherwise there will be errors. Use the default values ​​for other parameters, and then click OK to exit.
Click Add->Flash menu to pop up the hot air pad size setting dialog box, as shown in Figure 1.9.

Enter the inner diameter 40 in the Inner diameter edit box, enter the outer diameter 50 in the Outer diameter edit box, and enter the connection width 15 in the Spoke width edit box. It is best not to be less than the minimum line width of the board. Select the number of openings in the Number of spokes, the default is 4, and the Spoke angel input opening angle is the default 45 degrees. Other defaults, after clicking OK, a flower pad shape will be automatically generated, as shown in Figure 1.10.

At this point, a circular hot air pad is completed. If you want to generate other shapes of pads, such as oval, square, etc., you cannot use Add->Flash to generate it. You need to use the draw rectangle and circle tools under the Shape menu Come draw. First, draw a sketch by yourself, and calculate the coordinates of each point, and then use commands such as drawing rectangles and circles and enter the coordinates in the command status bar to draw. It should be noted that since the hot air pad is used in the negative film, the place you can see the shape is drawn (the area enclosed by the green line in Figure 1.10) is actually corroded after the PCB is made, and the black (bottom) Color) is where there is really copper.