Altium Designer Documentation

Add Shielding to Net

Modified by Susan Riege on Oct 23, 2018
This documentation page references Altium Vault, which is no longer a supported product. Altium Vault and its component management features have migrated to Altium Concord Pro.
All Contents


The Add Shielding to Net dialog

Summary

The Add Shielding to Net Dialog is used to add a shield to a net. A via shield is used to create a vertical copper barrier through the PCB to help reduce crosstalk and electro-magnetic interference in a route that is carrying an RF signal. A via shield, also known as a via fence or a picket fence, is created by placing one or more rows of vias alongside a signal route. 

Access

The dialog is accessed from the PCB Editor by clicking Tools » Via Stitching/Shielding » Add Shielding to Net from the main menus.

Options/Controls

Shielding Parameters

The shielding parameters control the shielding vias' placement pattern and their clearance from other-net and same-net objects.

  • Net to shield - net to have shielding vias placed around.
  • Selected Objects - place shielding vias around the selected objects rather than the entire net selected in the Net to shield field.
  • Stagger alternate rows - alternate rows of shielding vias are offset by half of the Grid value.  
  • Row Spacing - spacing between rows of shielding vias (edge to edge separation) when the Rows setting is greater than 1. 
  • Distance - separation from the edge of the shielded net track segments, to the edge of the shielding vias.
  • Grid - the distance between the edges of adjacent shielding vias. Shielding vias will not be placed in violation of applicable design rules; if a potential via site would result in a violation then that site is skipped.  
  • Rows - number of rows of shielding vias.
  • Add shielding copper - place a polygon over the area occupied by the shielding vias, connected to the net specified in the Via Net field. The polygon is defined in accordance with the applicable Clearance constraint and Polygon Connect Style design rules.
  • Add clearance cutout - include a polygon cutout around the shielded net, set back from the net by the distance specified in the Distance field. Use this when you require a different clearance from the applicable Clearance constraint design rule. 

Via Style

The shielding Via Style can be configured manually by selecting the desired style or can be imported from the applicable Routing Via Style design rule by clicking the Load values from Routing Via Style Rule button. Clicking this button will load the Preferred rule settings. 

Diameters

  • Simple - Via Style (Hole size and diameter) is the same through all layers.
    • Hole size - specify the hole size value for the Via.
    • Tolerance Min/Max - setting hole tolerance attributes can help determine the fits and limits of your board. Specify the Minimum (-) and Maximum (+) hole tolerance for the design.
    • Diameter - specify the diameter for the Via.
  • Top-Middle-Bottom - different Hole Size and Diameters can be set at Top Layer, Middle Layer and Bottom Layer.
    • Hole size - specify the hole size value for the Via.
    • Tolerance Min/Max - setting hole tolerance attributes can help determine the fits and limits of your board. Specify the Minimum (-) and Maximum (+) hole tolerance for the design.
    • Top Layer - specify via size for top layer.
    • Middle Layer - specify via size for Middle layer.
    • Bottom Layer - specify via size for Bottom layer.
  • Full Stack - different Hole Size and Diameters can be edited at each layer (including all signal layers and planes).
    • Hole size - specify the hole size value for the Via.
    • Tolerance Min/Max - setting hole tolerance attributes can help determine the fits and limits of your board. Specify the Minimum (-) and Maximum (+) hole tolerance for the design.
    • Edit Full Stack Via Sizes - click to open the Via Layer Editor dialog in which you can specify via settings for each layer stack.

Via Template

  • Template - select a via template from the drop-down.
  • Library - displays which library the via template is linked to and includes the option to Unlink the template from said library.

Properties

  • Drill Pair - the layers on which this via starts and ends.
  • Net - the net to which the via is currently assigned. Change the net assignment by clicking in the field and choosing a net from the drop down list. Select No Net to specify that the via is not connected to any net. The Net property of a primitive is used by the Design Rule Checker to determine if a PCB object is legally placed.
  • Locked - enable this option to protect the via from being edited graphically. Lock a via whose position is critical. If you try to edit a primitive that is locked, you will be informed that the primitive is locked and asked if you wish to proceed with the action. If this option is unchecked, the primitive can be freely edited without confirmation.

The Start Layer and End Layer settings define a via to be one of the following types:

  • Multi-layer (Thru-Hole) - this type of via passes from the Top layer to the Bottom layer and allows connections to all internal signal layers.
  • Blind - this type of via connects from the surface of the board to an internal electrical layer.
  • Buried - this type of via connects from one internal electrical layer to another internal electrical layer.

Solder Mask Expansions

  • Expansion value from rules - enable to allow the existing solder mask expansion rule to take effect on this pad object. Check the Mask design category from the PCB Rules and Constraints Editor dialog.
  • Specify expansion value - enable to edit the expansion value and the solder mask expansion design rule is overridden for this pad.
  • Force complete tenting on top - enable to override any solder mask settings in the solder mask expansion design rules and results in no opening in the solder mask on top layer of this pad. Disable this option and this pad is affected by a solder mask expansion rule or specific expansion value.

  • Force complete tenting on bottom - enable to override any solder mask settings in the solder mask expansion design rules and results in no opening in the solder mask on the bottom layer of this pad. 
    Disable this option and this pad is affected by a solder mask expansion rule or specific expansion value. 

Additional Controls

  • Drill Pairs - click to open the Drill-Pair Manager dialog which allows you to configure the required drill pairs for the active layer stack.

Tips

  • Each set of shielding vias are added to a union. The set can be removed by running the Tools » Via Stitching/Shielding » Remove Via Shielding Group command, then clicking on any via in the group.
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.

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.