If you want to create a footprint of an Integrated Circuit the IC Wizard of TINA can assist you.
Activate the IC Wizard from the Insert menu of the Footprint Editor of TINA PCB Designer. The wizard presents several properties of the IC which you can set.
In this tutorial video we will use the MAX11166 converter to show how to use the IC Wizard of TINA Footprint Editor.
Watch our tutorial video to see how to use the IC Wizard of TINA Footprint Editor.
Download the FREE trial demo of TINA Design Suite and get:
- One year free access to TINACloud (the cloud-based, multi-language, installation-free online version of TINA now running in your browser anywhere in the world.)
- An immediate 20% discount from the offline version of TINA
- Free license for your second computer, laptop etc.
You can also find below the script of the video:
Using the Footprint Editor in TINA, part 1: IC Wizard
Start TINA PCB Designer by using the Start menu of Windows 10
Click the Tools menu
Select Footprint Editor
First, select View
and change the Unit into mm and the Precision into 3
then click OK
Create a new Footprint Library by using the File
Save Library As command
in the Private Catalog Folder of TINA
under the name: MyPackage
Press the Save button
Click the Insert menu
Select IC Wizard
In the Technology group, you can set the mounting mode and the package type of the IC. The mounting mode can be through hole or surface mounted. Depending on the mounting mode the following packages are available: DIP (Dual in line packag e), PGA (Pin grid array package), SPGA (Staggered pin grid array package), SOP (Small outline package), LCC (Leaded chip carrier package), QFP (Quad flat package), BGA (Ball grid array package), SBGA (Staggered ball grid array package), SIP (Single in line package) and ZIP (Zigzag in line package) respectively.
In the Package dimension group, the dimensions (length, width,
3D height) of the package can be set. Depending on the selected package, the 4th parameter is either notch, corner cutoff, or ignored.
The Pad dimension defines the shape and dimensions (length, width)
of the pad. If the mounting mode is through hole, the shape of the
drilled pad can be round, square or octagon. Moreover, the shape
and dimensions of the drill diameter can be defined.
However, if the mounting mode is surface mounted, the shape of the pad
can be circular, rectangular or rounded corner and the appropriate
dimensions can be also set.
In the Pad position, the number of pins and the distances between them can be set according to the package type.
Finally, in the Pad numbering group, the type and direction for pad numbering can be entered, depending on the package type.
Set the data as shown in the IC Wizard window above
In the pop-up window the following message appears:
You can enlarge the image by using the Zoom option
Next, we will position the Smd Pad
Click the Smd icon, then click on the Editor workspace to place it
Double-click the SMD Pad
and in the SMD Pad Properties Window enter 13 in the name field, 0 in the Center X and Center Y fields
Double-click the Size field and enter 2.5 in the Width and 1.7 in the Height fields
Click OK again
We will now position the labels which belong to another layer
Click the little arrow next to the TOP layer icon and select the Silkscreen Top layer
Now you can easily move the Name and the Value labels by holding down the left-mouse button while dragging them
Select again the Top layer when you are done
Click the New Footprint Group icon
Click the <New group> folder and rename it by entering the name: SON then press the Enter button on the keyboard
Note: SON is small-outline no leads type of circuit
Click the Footprint Properties icon
and in the Name field enter: SON12_3x3_12_0.5TP
Click the Add Footprint to the library icon
Save the footprint by clicking the Save button
Close the Footprint Editor
You can check the newly created Footprint
Reopen the Footprint Editor
Open the MyPackage.FPL
Next, double-click the SON library, then the new Footprint
The mapping between TINA’s Schematic Symbols and the Footprints used in TINA’s Integrated PCB Designer will be presented in another video.