Custom Pad Creation - Multiple Pad to Single Pin

Modified by Admin on Jun 4, 2021

Custom Pad Creation instructions, as well as explanation of single schematic pin assigning net to multiple PCB Pads with same designator

Applicable Versions: 17, 17.1, 18, 18.1, 19, 19.1, 20, 20.1

Solution Details

Custom Pad Shape Creation
 

Custom pad shapes are created by placing other design objects, such as arcs, fills, lines, or regions to build up the copper shape required for the pad. Placing a small Pad within the shape is required to define the connection point in the pad, and if required, the drill hole location and size. 

Any design object can be used to build up the required copper shapes needed for the pads. Choose the object to suit the shape required. In this example, the use of a simple Solid Region is shown.
 

Within a .PcbLib Footprint Creation/Editing environment

File ► New ► Library ► PCB Library
 

 

Place ► Solid Region
 


 

Create your custom shape using the these Tips:

  • Press Shift+Spacebar to cycle through the corner modes
  • Press Spacebar within each corner mode to toggle the corner direction (except for the Any Angle mode). 
  • Press Backspace to remove the last corner.
  • Press Esc or Right-Mouse Click to terminate the placement process, the software will close and complete the Region.
  • For the Arc Corner Modes, the Arc can be Resized using the ‘,’ and ‘.’ keys. Hold Shift to accelerate the re-sizing process.

 

See Also

Region -

https://www.altium.com/documentation/altium-designer/pcb-obj-regionregion-ad

 

 

Solder and Paste Mask

 

Any primitive object can have a calculated Solder and/or Paste Mask, which can either be a user-specified amount or controlled by the rule system. This is achieved enabling the appropriate Mask Expansion settings in the Properties panel when the primitive object is in selection, as shown in the image below.

 

 

 

Creating Connectivity

 

In order to create a Pin to Pad pad connection via Pin Designator in the schematic and define the connection point in the pad; a small pad must be placed into the region with the designator set accordingly to match the pin designator of the pin in the schematic symbol for which the footprint where the custom pad being used is attached.

 

Place ► Pad ► ‘Tab’

Set the properties of the Pad accordingly in the Properties Panel

In this case the Properties of the Pad are set to:

  • Designator: 1
  • Layer: Top
  • Shape: Round
  • (X/Y) 30mil
  • Paste Mask Expansion: Manual - 0mil
  • Solder Mask Expansion: Manual - 0mil

 

 

A Pad is placed in each section of the Region where there is need for Hotspot connection for Tracks and Spokes of a Thermal Relief. All pads in a footprint with the Designator of 1 will inherit the net assigned to the Pin with a Designator of 1 in the schematic symbol for which the footprint is attached to. To ensure the small pads are connected by spokes of a Thermal Relief connection, position them close to the edge of the custom shape so that the distance from the small pad edge to the edge of the custom shape is less than half the polygon connection spoke width.

 

 

 

If a Drill Hole is required; change the property of the internal pad to Multi-Layer and define the Hole Size accordingly in the Properties Panel.

 

 

 

See Also:

Working with Custom Pad Shapes -

https://www.altium.com/documentation/altium-designer/working-with-custom-pad-shapes-ad

Creating the PCB Footprint -

https://www.altium.com/documentation/altium-designer/creating-the-pcb-footprint-ad

 

 
 
 
Was this article helpful?
0
0
Found an issue with this document? Highlight the area, then use Ctrl+Enter to report it.

Contact Us

Contact our corporate or local offices directly.

We're sorry to hear the article wasn't helpful to you.
Could you take a moment to tell us why?
You are reporting an issue with the following selected text
and/or image within the active document:
ALTIUM DESIGNER FREE TRIAL
Altium Designer Free Trial
Let’s get started. First off, are you or your organization already using Altium Designer?

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

In that case, why do you need an evaluation license?

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

Got it. You actually don’t need an evaluation license for that.

Click the button below to download the latest Altium Designer installer.

Download Altium Designer Installer

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

Please fill out the form below to get a quote for a new seat of Altium Designer.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

If you are on Altium Subscription, you don’t need an evaluation license.

If you are not an active Altium Subscription member, please fill out the form below to get your free trial.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Why are you looking to evaluate Altium Designer?

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

You came to the right place! Please fill out the form below to get your free trial started.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Great News!

Valid students can get their very own 6-month Altium Designer Student License for FREE! Just fill out the form below to request your Student License today.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Got it. You can download a free Altium Designer Viewer license which is valid for a 6 months.

Please fill out the form below to request one.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

That’s great! Making things is awesome. We have the perfect program for you.

Upverter is a free community-driven platform designed specifically to meet the needs of makers like you.

Click here to give it a try!

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

Got it. You can download a free Altium Designer Viewer license which is valid for a 6 months.

Please fill out the form below to request one.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.