The DIP14/300 (where /300 signifies the pin to pin distance) package, as
shown in the figure below, may be created using the following steps.
1. Double click
Library in the Project Explorer to launch the Library Editor. To
start creating a new package, click the tab PACKAGE to open Package Editor.
2. Select File / New Package. A single pin with Component name, Component
description and User reference appears on the workspace. This entry is located
at X, Y location 0,0 and its first pin. Each pin of the physical component has a
specific size. To assign this size information, we will have to specify a
padstack for each pin. Select the Function tool Properties and click on the
enrty. Click Add new padstack column and browse necessary padstack . drop down in the property window, select the required padstack.
3. Choose an existing padstack P_RND_50_H_35 and click Accept selection. Now from Change Padstack's drop down in the property window, select the required padstack.
Tip: We may view the actual size of the pin by choosing View | Package | True Size.
4. Select the
Repeat Item function tool to repeat the pads. Select Step Repeat item option tool to repeat it in steps. Click on the center of PAD/ PIN already positioned. The
Step Repeat menu will appear and it prompts for the inputs viz. steps, dx, dy. Since DIP14/300 contains 14 pins placed equally on either side, we enter the following information
6, 0, 0.1. Click OK to place pads on one side vertically upwards with the difference of 0.1 inches.
5. Now we will start the second row of pads for the IC. Unselect
Step Repeat Item, click on the 1st pad and then move the cursor by the inter-pad distance (for DIP14/300 it is 0.3000”) and place the 8th pad.
6. Now we may repeat the above step to create another 6 pads of the DIP14. Click on the eighth padstack. The dialog box appears. Type
6, 0, -0.1. We will find another set of 6 pins have been created.
7. All 14 pins of the IC are placed. We have to create an outline for the part. The outline should be on the Comp.Print layer in board design. Hence this rectangle must be created on this layer. To select the layer on which to create drawing items, go to
Layer | SelectLayer | Comp. print or simply select COMP.PRINT from
Layers toolbar (Toolbar can be displayed by View | Toolbars | Layers). This will set the layer as COMP.PRINT for creation of graphic elements.
Create Graphic Item tool and then
Create line option tool to create a rectangle border around the pads. Now turn ON the grid, and set the grid and snap size. Click on the workspace. A small line will appear at the cursor. Move the cursor to the point where the graphic should start and press the left mouse button. As we move the cursor, the line is stretched, left click on completing one side. Refer picture below and create the lines 1-2, 2-3, 3-4,5-6 and 6-1. As per the general convention usually a small curve is present in the outline to identify the starting point of pin numbering. Place contact points on 4 and 5 and create an arc on the outline using the tool
Create Arc as shown below.
9. The IC’s first pin is generally a square pin. This is to help identification for assembly. We will then have to change the shape of pad for pin 1. Change the padstack assigned to this pin from P_RND_50_H_35 to P_SQR_62_H_35. Select the
Function tool Properties and click on the enrty. Click Add new padstack column and browse necessary padstack, here it is P_SQR_62_H_35 .Click Accept Selection will return to the workspace with the padstack replaced. Pin 1 is now a square pin.
10. Enable the
Relocate function tool and click on the COMP NAME text. We see that the text gets tagged to the cursor. Drag and position it near the top of the symbol at the left top corner. This defines the position for the component designator in the layout.
11. Select File menu | Save Package and save it to a disk library.