We will see together how to create a basic footprint (named Decal) with PADS Layout.

We will create the CK05 Decal like this:

From the main PADS Layout menu, select [ Tools ] then [ PCB Decal Editor ] commands...

Select [ Tools ] then [ Options...] commands...

Before drawing the Decal, select in this dialog box units that you want to use (Mils, Metric or Inches).

In the same Dialog box, select the "Grid" Tab to enter "Design Grid" and "Display Grid" values. Each item of the Decal like pads, lines, texts, etc. will be placed with the mouse on the "Design Grid". The "Display Grid" is the visual grid (white points in the display). Values of the "Design Grid" and "Display Grid" can be differents.

Ok, we are ready to draw the Decal. First of all you can see : origin (a big white dot), "Name" and "Type" texts. "Name" is the location of the REF-DES (U1, C1, etc.) in the design. "Type" is the location of the Part Type (7400, CC1210, etc.). We will move them later.

The first step is to add pads. Select the [ Drafting Toolbar ] the [ Terminal ] commands...

Move the mouse on the origin then click on the left mouse button. The first pad numbered "1" is added.

Move the mouse at 200 mils to right the press then left button again. A second pad, numbered "2" is added. How to know if the location of pad is correct ? When you move the mouse, the XY location is displayed in the right bottom of the window.

The second way to add a pad is to use the "Modeless Command". Click on the [ Terminal ] command. Press the "S" key. A little dialog box is displayed. Enter X space Y value then press "Return". The cursor move to this location...

Press the space bar to add a pad. The "S" command (for Search) can be use to enter XY location with the keyboard with more accuratie. There is a difference between adding a pad with the mouse and by using the "S" command. With the mouse, any pad can be place only on the "Design Grid" only. For example, if the value of the "Design Grid" is 25 you can add a pad only on 25 increment. If a pad is not on a 25 increment you must change the "Design Grid" value. If you enter pad with the "S" command you can add a pad with the value entered even values are not "Design Grid" increment.

Select the [ Select ] command...

Click on right mouse button. Select the [ Select Terminals ] in the popup menu. With this action we can select only pads.

Click the pad "2" with the left mouse button. The pad is selected. PADS Layout displays the selected pad with the white color.

Click on right mouse button. Select the [ Pad Stacks...] command in the popup menu. This command allows to define pad.

The "Pad Stack Properties for Pin" dialog box is displayed. Use it to define geometry, sizes and drill for each pad.

If you select all pads...

(then click on right mouse button and select the [ Pad Stacks...] command in the popup menu)

All pads are displayed in the "Pin Name: Plated" list. You can define all pads.

Zoom in the screen. Select now the [ 2D Line ] command...

Select "<All Layers>" to draw the outlines of the Decal. Why ? PADS Layout uses "All Layers" for outlines.

Click on the right mouse button then select the [ Path ] command in the popup menu to draw line segment.

Add two lines like this:

Click on the [ Select ] button...

Click on the right mouse button the select [ Select Text/Drafting ] to select "Name" and "Type" texts.

Select each text and move it like this. It is important to place correctly "Name" and "Type" in the Decal to avoid to move them in the design after... for each CK05 Decal!

The drawing of the CK05 Decal is complete. To save it in the library select [ File ] and [ Sace Decal As...] commands.

Select library and Decal name in this dialog box...

PADS Layout purposes you to create the Part. For this sample click on the "Yes" button. Why ? You can create a design without any schema (and PADS Logic) but to add a Decal in a design, PADS Layout add... a part not a Decal. To use this feature when you create a Decal, PADS purposes to create the associated part immediately. If you use PADS Logic you have created symbol and the part before.

It's done. You can leave the PCB Decal Editor. Click on the [ Exit Decal Editor ] command to leave it and go back to the design window.