If you need to customize the paste mask on your thermal pad, you can do this easily by moving your standard calculator-built part into the Footprint Expert FP Designer module.

The SMD Calculators only produce rectangle shape thermal pad paste mask.

You can fully edit pad stacks in FP Designer.

Use the Calculator to produce the master pattern used for the 3D STEP model.

Move the Calculator footprint to FP Designer.

Select the Pad Stack Manager

Edit the thermal pad stack > paste mask > radius > Save Changes > Close

Edit Specifications > enter manufacturer name > case code > OK > Finish > Add to FPX

The Footprint Expert's "FP Designer" module can automatically build BGAs with up to 99,999 pins by importing CSV files.

You can import this .TXT file into FP Designer:

INTEL_BGA-1296-Pad_Placement.zip 

(or see online version here)

Creating Staggered Pin BGAs can be tricky. There are a couple ways:

BGA with Alphanumeric Rows:

 

BGA with Alphanumeric Columns:

 

You need the package dimensions for Length, Width and Height. For this demo we'll use 7, 5, 2. You'll also need to know the Pin Pitch and Pad Diameter. For this demo we'll use 0.75 and 0.40.

Select the "Designer" button and insert the package dimensions.

 

Select the OK button and the Drafting Outlines for Silkscreen, Assembly, Component, Courtyard and Origin will be auto generated.

 

The Pad Stack Designer will automatically appear. Create a Round surface mount pad 0.40 diameter and select "Add Pad Stack to Design Queue" and then "Add Queue to Design".

 

The Pad Stack Manager will automatically open to allow you to edit the pad stack layer sizes and shapes. If there are no edits, select "Save and Close".

 

In the Define Placement menu select the "Open Wizard" button. When you enter simple values in the Wizard for Pin Count, Pin Pitch and Offset. Select "Apply Wizard" to populate the X/Y coordinates in the Pin Placement menu. Then enter the X Stagger dimension and enter "A" in the Alpha pin options. You will see an Example of the Alphanumeric Pin Assignments.

Select the "Open Wizard" button

Select the "Add To Design" button

The pads will display in the Footprint Viewer with Alphanumeric Rows

For Alphanumeric Columns select the Undo button

Then select the Pin Array Wizard Pin Direction to Column (Blue highlight)

The new values will auto-populate the Pin Options cells. See the Example Pin Assignments.

Select "Add To Design" button

The pads will be added to the footprint in alphanumeric columns

Add the footprint to your master FPX file and export to any CAD format.

The BGA pin quantity limit is 99,999 pins.

You can build any staggered pin BGA in minutes using the Pin Array Wizard

You can create any footprint, regardless of the complexity, in just minutes using Excel and a Text file. The ability to transform a simple text file into an accurate solder pattern is available in Footprint Expert. The text file can be easily created in Microsoft Excel or Google Sheets, and must contain these features to fully automate PCB library construction:

Note: The Pad X, Y and Diameter data is for the creation of surface mount pad stacks. 

Tip to automate the Pin Names, enter the first Pin Name in cell A1

After Click and Drag, Excel will step the pin numbers

Next, add the pad rotation. Pad stacks are usually created long in the horizontal or X direction. If only one rotation is required, enter the angle in cells B1 and B2 and select both cells.

 

After Click and Drag, Excel will add the pin rotation

Next, enter the X coordinate in cell C1 and the step value in cell C2

After Click and Drag, Excel will add the X coordinates and step the values according to the difference between cell C1 and C2. 

 

Here is a Molex Surface Mount USB Type B Connector P/N 47346-1001 Datasheet:
https://www.molex.com/pdm_docs/sd/473461001_sd.pdf 

Capture 3 dimensions for Length 7.5, Width 5 and Height 2.45

Create an Excel spreadsheet with the Mfr. Recommended Pattern X/Y coordinates and pad sizes and Rotations. The footprint Origin is in the center of the component package. 

The Excel spreadsheet contains Pin Number, Pad Rotation, X & Y placement Coordinates and X & Y Surface Mount Pad Stack sizes. Using the Mfr. Recommended Pattern, it takes 5 minutes to create this. Every component manufacturer should provide this file to all their customers to automate accurate PCB footprint creation. Using Footprint Expert, this PCB library part can be created in 2 minutes and exported to 25 CAD tools. 

Select File > Save As > Tab Delimited (Excel) or Tab Separated (Sheets) text, and save as a .txt file. If you view the TXT file in Notepad, it will look like this:

Open Footprint Expert, select "Designer" and enter the package dimensions for L, W and H.

Select OK and Footprint Expert will auto-generate the Silkscreen, Assembly, Component, Courtyard and Origin drafting outlines. Entering 3 dimensions takes less than a minute.

After selecting the OK button, the Pad Stack Designer menu opens. Close it because the text file will auto-generate all 5 pad stacks.

Open the Import Placement panel and search for the .txt file on your computer.

Mouse over the Yellow Highlighted Headers and a message appears "Right-click to select a definition for this column".

Select the proper function for each column from the pop-up list.

Do this for each column and then select and Confirm Units.

Select Units, Confirm Units and Add to Design

 

Here is the footprint with the proper pad stack location, size and rotation for 5 different pad stacks.

The Silkscreen Outline is auto-trimmed per your personal Option settings, the Assembly Outline has a Pin 1 Polarity Chamfer and the Placement Courtyard auto-sized and contoured around pads.

Save the footprint to your Master FPX file and output to any CAD format!