Basic Terminologies

Grid: Graphical aid for placing the component
Snap: The minimum distance that the cursor can jump from one position to another position with an object tagged to it.
Angular Snap: The minimum angle that the cursor can jump with an object tagged to it
Entry Point: The point at which the electrical connection given or taken to/from th e component pin.
Pad: A circular/ oval/ rectangular/ line shaped seat for component pin with necessary diameter and hole (optional) created with copper.

Units
1"=1000mils
1"=25.4mm
0.1"=2.54mm=100mils
From View choose Units → inches
Set Grid as 0.1" and Snap as 0.05"

Naming Conventions

Packages in EDWinXP are named in the format Package type No: of pins in the package/horizontal pitch between the pad in mils. Eg: DIP14/300 where DIP is the package type, 14 is the no: of pins in the package and 300 is the horizontal pitch between the pads in mils.

To create a library part first you need to create the symbol and package of the part. Part constitutes of Symbol and package.

Library creation Using Wizard

Open EDWinXP Main from Start →Programs → EDWinXP → EDWinXP Main. Choose Library right click Library and choose Library Editor.

Creation of Symbol

View Video

For creating symbols automatically, select Symbol tab / File/New Symbol using Wizard from Library Editor. This utility provides an easier interface for creating s ymbols. The Symbol creation wizard is as shown in figure below.

1. Specify the name and type of the symbol. For eg : Specify the symbol name as 7408 and symbol type as general symbol. Click on Next button to move to the parameter specification window.

2. Specify the parameters, the description about the parameters that is to be specified while creating the symbol for 7408 is given below. Click on Next button, a new window appears which specifies the orientation of all entries, whether or not they are invertible, invisible etc.

No: of Entries (n) :3
Entry placement grid (P) :.1000’’
No: of Pitch for terminal line length (nP) :2
Orientation of entries : Auto

Positions
Component name : Top
Component description : Top
Line Size : .0020’’
Symbol Type : Double click on the field, Select Digital→Gate →AND from the drop down menu.
Symbol Description : AND Gate

Check display entry names as text check box.

3. In the new window edit, the entry name attributes. You can also indicate the swap level and Sim Name. An import pinlist option is also available.

The Pin details format should be like Pin-Number, Pin-Name, Pin-Orientation (valid PinOrientations are *Left ( L ), Right (R),Bottom (B),Top (T). Any invalid format will produce error in operation. Comments should start with a '*' character.

Window after importing the list is as shown below.

4. Click on Next button moves to a new window where the pitch between two entry pins can be specified.

For example if the pitch between the pins has to be changed to 4 then give 1, 2, 4 in the field allowed for entering and click on the up arrow and then click on the arrow directed to right. Then the pitch between the pins is changed as applied.

Click on Next button moves to a new window, which displays the summary of information about the symbol created using the wizard.

5. Click Finish to complete the process.

From the File Menu choose Save Symbol As. In the new Window Set the Symbol Name and the Lib Name.

Check On top of search sequence check box and Save.

Creation of Package

In order to create package, click on Package tab.

View Video

1. Select New Package using Wizard from the file menu for creating the package for example IC7408.
2. Set the Package Name as DIP 14/300, 14 denote number of pins in this package and 300 denotes the width of the package. Package Type as Dual In Line Package (DIP).

3. Click Next button to continue.

In the Window, which appears, enter the following values

No. of pins : 14
Pin to pin Distance : 1000”
Horizontal pitch between pads : .3000”
Length of Package outline : .7000”
Width Package outline :. 2000”
Package Description :AND GATE

4. Padstack is selected by double clicking on the field Default Padstack, a window for selecting padstack is displayed as shown in figure below. From the menu select the padstack and click Accept Selection. Then automatically the padstack name is assigned to the required field.

5. Package Type is given by double clicking on this field, a window for selecting the package type is displayed. From the drop down menu select PMD →DIP → DIP Narrow. Click Accept.

6. Click Next, Change the Pad Name of first pad (#1) to P_SQR_55_H_30.

7. Click Next.

8. Click Next.

9. Click Finish.
10. From the File Menu choose Save Package As.
11. Give Package name as DIP14/300 and Lib Name as Sample
12. Check On top of search sequence check box and Save.

Creation of Part

View Video

1. Click on Part Edit tab, enter the Part and Package details as

Part details

Name : 7408
Description : AND Gate

Select manufacturer, technology and type from the drop down menu by double clicking on the required field.
Manufacturer : Fairchild
Technology : TTL
Type : Digital→Gate→ AND

Package Details

Package : DIP14/300

Click Yes for the question “Are you sure to change the package?”

Select Package type by double clicking on the field and select PMD →DIP →DIP Narrow.

2. From the Edit Menu choose Add Group, In the new window, Give 1, 7408 (Symbol name given during creating symbol). Similarly add 3 more groups by repeating Edit →Add Group.

3. After adding four groups, Choose Edit →Edit Pinout. In order to view assigning each group to the package select Edit →Show Package Window.

4. Choose Edit →First group and assign first group to the package by clicking on the Entry field. Select inputs and output pins according to the package.

5. Select Edit →Next Group to assign the second group to the package. Name Pin no: 7 as SPL0 and Pin No: 14 as SPL1. Assign groups third and fourth similarly as done early.

6. Select File → Save Part, give Part Name as AND and Lib Name as Sample.

7. Check On top of search Sequence check box and Click Save.

Creation of Padstack

1. Select File | New Padstack using Wizard. to pop up window as shown in figure below.

2. In the window, a miniature representation of the padstack is shown in the preview. Right click on the preview for options to view True size, Hrf items and Airgap view. From the Fetch from Padstack Library(s) tab, select the padstack “N_RND_100_H_100”. Now on moving to the Edit or create new padstack tab, the padstack details of “N_RND_100_H_100” appears.

3. The minimum information required to create a New Padstack is given in the figure below. The user may edit the values.

Name = N_RND_100_H_100 and press the < enter > key.
Create HRF items = select the checkbox
Airgap = 0.0120"
Hole Category = 0
Hole diameter = 0.1000"

4. On clicking the Edit by layers button, the pad details of different layers (Shape, diameter, Airgap and the option of selecting the layers to be used) appears.

Global Editing of layers is also allowed.

5. Finally click the button Make to create the new padstack. Now the edited changes are visible in the Preview in the right pane. Click on Proceed to manual editing to effect the changes and exit.

This completes the Padstack creation using wizard. The edited padstack appears in the Padstack editor and further edition can be done using the tools availabl e.

Library Creation without using Wizard

Open EDWinXP Main from Start →Programs→EDWinXP →EDWinXP Main
Choose Library, right click Library and choose Library Editor.

Creation of Symbol

1. From Library Editor choose Symbol tab at the bottom of the page.

2. To create a symbol of OR gate, select the Set Contact Point (function tool)→ select the first option tool and place it on the grid. Similarly select the second one and place it on the next grid as shown.

3. Select the Create graphic item (function tool) → Create arc (option tool). Click anywhere near the contact point to get an arc tagged to the cursor.

4. After adjusting the size of the arc, click to place it. Adjust the arc, if necessary, by selecting the Stretch Item function tool and click the Stretch arc radius tool or press F1 key, to change the radius of the arc.
5. Repeat the arc as needed, after placing the arc press ESC.
6. Select Create line and click on the workspace where the line needed.

7. Repeat the same line using the tool Repeat Graphic Item, select this tool and click on the workspace then a line is tagged with the cursor, place it where required.
8. Place the first/default entry (+) present in the workspace, exactly at the starting point of the first pin of the OR gate using the Relocate item tool.
9. Select the Create graphic item tool and click the Create entry pin option tool or press F6 key, for creating the remaining entry points. Click on the starting point of the pins.

10. From the File Menu choose Save Symbol As

11. In the new Window.
    Set the Symbol Name and the Lib Name
    Check On top of search sequence check box and Save

Creation of Package

From Library Editor choose Package tab at the bottom of the page.
Select the Component Print, by default component layer will be selected.
To create the outline of the package, select Create Graphic Item (Function tool) →Create rectangle (Option tool).
Place the first/ default pad (+) exactly at the place of the first pad using the Relocate item tool.

For placing the remaining second pad select the Create graphic item tool and click the Create Pad option tool.

The pad is placed at the required position and displayed as a small “x”. To change the padstack, click Change Padstack tool and select Select Padstack option tool.

Select an SMD pad, Eg: Select S_RCT_40*48 SMD pad.

Click Edit or create new padstack tab →Edit by layers tab to edit the shape and size of the pad.
To reflect the changes made in the selected padstack click button.

Click the Accept Select button to select this padstack. Click on the center of each pad to locate the pads made.

From the File Menu choose Save Package As.

Give Package name as OR Gate and Lib Name as Sample.

Check On top of search sequence check box and Save.

Creation of Part

Same as in the creation of part using wizard.