How to Use Altium Designer to Quickly Create a Component Footprint

March 2, 2018 Altium Designer

Footprint in the shape of a chip

 

 

When laying out your PCB, it is critical that you use the correct footprint for your part. Failing to do so will cause problems with the manufacture or operation of your board. If the footprint is incorrect, the part pins may not align with PCB pads or the part may violate clearance or spacing rules that could lead to significant loss of time and additional cost.

 

When designing your PCB you can sometimes rely upon a program part library to provide you with an accurate footprint for your part. However, this is not always the case and invariably you will at some point have to create your own footprints. With some PCB software packages, this can be a difficult task that comes with a steep learning curve before you become proficient. With Altium Designer, on the other hand, you can quickly create a component footprint.

 

Steps to Create your Component Footprint

Creating your footprint in Altium Designer consists of 3 steps:

  1. Create the pads
  2. Add silk screen information
  3. Save the footprint

Let’s step through the process to see how easy it can be to create your component footprint.

 

Here’s how to create your footprint in Altium Designer in 3 easy steps:

Step 1: Create the Pads

You will need the landing pattern for your part, which can be found towards the end of the component data sheet. For this example, let’s use the popular PIC24FJ64GA004 microcontroller.

 

Component Landing pattern illustration and dimensions

Component landing pattern

 

In Altium Designer, under File click on New, then Library, then PCB Library to create a new PCB component library.

 

Open PCB Library window

Open PCB Library window

 

 

The first thing we need to do is set our units. Units are listed in the upper left corner of the window. The datasheet for the part only has dimensions in mm. If the dimensions given are in mil, then under the View menu click on Toggle Units to convert to mm.

 

Click on the pad icon on the PCB Lib Placement toolbar at the top of the window (or click on Pad on the Place drop down menu to get a pad. Place the pad near the middle of the window (we will set this in a moment). Now, right click on the pad and select Properties. First set the Designator (pad number) to 1. Next, scroll down to Size and Shape, set the shape to Rectangular and the pad dimensions (X/Y) to 1.5mm/0.55mm. We will use this pad to map out our component footprint.

 

Pad 1

Pad 1

 

Now, we create an array of pads for a side of the footprint by copying and pasting. (Tip: Select the pad(s) first then click on the Copy icon. To place, just click on the Paste icon.) We need to make sure that the vertical distance between the pads is accurate.

 

One way to do this is to set the Global Snap to Grid value, which can be accessed from the View drop-down menu under Grids. Let’s use 0.2mm, which means there should be 4 windows between the vertical centers. To make sure that the pads in our array are aligned accurately we select the array, then click on the Edit menu and select Align, then Align Vertical Centers.

 

 Pads 1-11

Pads 1-11

 

The array of pads above can be either on the left or right side of the component footprint. If for the left side, they should be numbered 1-11 (top to bottom). If for the right 23-33 (bottom to top) (Tip: this is a convenience you will appreciate when linking to your schematic symbol to ensure that the pins and pads are properly aligned).

 

Next, we create the array for the opposite side by copying the array and pasting it 11.4mm away at the same vertical level. Be sure to set the pad numbers for the new array.

 

Right and left side pad arrays

Right and left side pad arrays

 

Now, we need to create the top and bottom pad arrays. Since our component has QUAD package, the number of pins and dimensions for the top and bottom are the same. We can take advantage of this to easily create the other pin arrays by simply copying both left and right side arrays at once, pasting them, and rotating by 90°. Don’t forget to set the pad numbers.

 

All pad arrays

All pad arrays

 

Step 2: Add Silk Screen Information

For this step, we add the silk screen layer image and pin 1 marking. We will follow the suggestion from the data sheet and indicate only where the corners should be. To make a corner, we create a 0.08mm line which you get by selecting the line icon on the PCB Lib Placement toolbar, duplicate it (by copy and paste) and link them.

 

You will need to rotate one of these by 90°. To do so, click on the Edit drop-down menu, then Move and then Rotate Selection. In the dialog, set the Rotation Angle (degrees) to 90. For the pin 1 marking, we will use a circle, which you can also select from the PCB Lib Placement toolbar. There is no need to make this too large, we only need this to be visible. (Tip: If you need to add labels or pin numbers, this is where you would add them).

 

Full component footprint

Full component footprint

 

Step 3: Save the Footprint

The final step is to create your component library is to name and save it so you can add it to your component library, which also includes the schematic symbol. Tip: You will want to make the name unique and searchable so you can easily locate it.

Additional Tips

The steps above illustrate a quick and easy way to create a component footprint using Altium Designer. Here are a few tips you may find helpful, as well.

 

  • When you open the PCB Library window, check to see where the view is centered. You can determine this by looking at the dimensions as you move the cursor around. It is a good idea to center the view where you want the center of your component footprint to be.
  • If it is not on, you may want to make the grid visible. This is helpful to visualize distances. If necessary, you can set the grid dimensions by clicking on the grid icon on the top menu.  
  • Check to see if your component’s package already exists in the database of component libraries. To do this, click on the Panels tab at the bottom right then open the Libraries dialog. From here you can search the available component libraries with footprints.  
  • If you would like a walk-through guide to help you create a component footprint then try either the PCB Component Wizard or the IPC Compliant Component Wizard. You can launch either of these from the Tools drop-down menu.  

PCB Component Wizard

Access PCB Component Wizard

 

Creating footprints for your PCB can be a painful process. Incorrect pad size, pad shape or clearance can lead to designs that cannot be manufactured and require a redesign that will increase your product development time and cost. Altium Designer makes it simple to quickly create component footprints to prevent these issues. You can follow the three simple steps give above or step through the process using one of Altium’s PCB component wizards.


For more information on how you can create a part footprint for your PCB design, contact an Altium PCB design expert. Or check out the Altium Resource Hub for more information.  

About the Author

Altium Designer

PCB Design Tools for Electronics Design and DFM. Information for EDA Leaders.

More Content by Altium Designer
Previous Article
Using PCB Star Grounding Can Keep Your Design Shining
Using PCB Star Grounding Can Keep Your Design Shining

Signal integrity, voltage concerns, and power distribution network management are vital to your PCB design’...

Next Article
PCB Layout Tips for Hall Effect Applications Keep Your Designs Positive
PCB Layout Tips for Hall Effect Applications Keep Your Designs Positive

By enabling magnetism and the Hall Effect within your PCB designs, you can make better usage of voltage and...

Get My Altium Designer Free Trial Today or Call 1-800-544-4186

Get Free Trial
×

Enjoying our blogs? Subscribe to our mailing list to have a weekly Altium blog digest sent to your inbox.

First Name
Last Name
Country
Acknowledging Altium’s Privacy Policy, I consent that Altium processes my Personal Data to send me communications, including for marketing purposes, via email and to contact me by phone.
!
Thank you!
Error - something went wrong!