Add Ground Vias

1Introduction

Add Ground Vias automates the placement of ground and stitching vias in Siemens Xpedition. It is built for RF and high-speed designs, where ground vias need to follow signal traces, fence the edges of copper pours and route borders, and fill pads — all at spacings derived from the signal's wavelength.

Beyond placing vias, the tool calculates recommended via spacing from your operating frequency and the board's dielectric constant, lets you tag groups of vias with a named property so they can be re-selected or removed later, and can add solder mask clearance and plane obstructs along selected traces. Everything is done inside your open Xpedition design, in a single transaction so it can be undone as a unit.

This guide is written for a first-time user. It walks through every region of the window, explains what each control does, and finishes with step-by-step workflows for the most common tasks.

2Requirements and Setup

Before launching the tool, make sure the following are in place:

• An Xpedition PCB session is open with your board design loaded.
• A valid ExactCAD license has been applied using the ExactCAD Licensing tool. The window title bar shows the licensed user name and the license expiration date.
• The design contains the via padstacks and layer spans you intend to use. The tool reads these automatically from the design.
• The design has a Config folder beside the PCB file. This is required, and is where the tool stores its list of via property names.

The tool detects your design's measurement units automatically and displays them near the bottom of the window. Length fields accept values in thousandths of an inch, inches, millimeters, or microns, with a units selector beside each one.

3The Application Window

The window is organized into several working regions. Becoming familiar with this layout makes the rest of the guide easy to follow.

• Left column: the parameters that describe the via and the trace it follows — the nets, the via to place, its hole and pad sizes, the trace width, the trace-to-plane gap, and the resulting lengthwise and crosswise via spacing.
• Upper right — Spacing Calculator: enter a frequency and dielectric constant and the tool reports the wavelength and several fractions of it, the signal velocity, and a plain-language spacing recommendation.
• Center — action buttons: buttons that place stitching vias along traces, around route borders, and into pads, together with the layer-span, design-rule, and density options that govern them.
• Center group — Fill Planes, Shapes, Obstructs, and Polygons: options for ringing or flooding copper shapes with vias.
• Lower left — Add Trace Features: tools to add solder mask clearance and a plane obstruct outline along selected traces.
• Bottom strip: the via-property tools, the current units display, the window options, the save button, and the status line.

4Via and Trace Parameters

The controls down the left side describe the signal you are stitching and the via you want to place. Most of them fill in automatically as you pick a net and a via, but every one can be edited by hand.

5The Spacing Calculator

The calculator in the upper-right of the window converts an operating frequency and a dielectric constant into a wavelength, and from there into the recommended via spacing. It updates as soon as you change any input.

5.1 Inputs

5.2 Calculated Readouts

From those two inputs the tool reports the wavelength and several useful fractions of it, all expressed in your design's units:

The wavelength is found from the relationship λ = c / (f × √Er), where c is the speed of light and f is the frequency. The velocity of propagation is c / √Er. A higher dielectric constant shortens the wavelength and slows the signal, which is why both inputs matter.

5.3 Recommendations

The recommendations panel restates the result in plain language. It reports one fifth of the wavelength for your frequency and dielectric constant, then advises that the maximum via spacing along the trace should not exceed that amount plus the via diameter, and that the vias across the trace should sit as close to the gap as possible without the pads intruding into it. These two figures are exactly the lengthwise and crosswise separations shown on the left side of the window.

6Via Span, DRC, and Density

These options control which layers the vias connect, whether placement respects design rules, and how tightly the vias are packed. They apply to the via-placement actions described in the next sections.

7Adding Stitching Vias

Three actions place stitching vias in the most common situations. Each one acts on what you have selected in Xpedition, using the via, span, and spacing settings described above.

7.1 Adding Vias Along a Trace

This is the core function of the tool. Select one or more traces in the Xpedition window, then use Add Stitching Vias to Trace. The tool walks each selected trace and places ground vias along both sides at the lengthwise and crosswise separations shown on the left. Nets that form a differential pair are recognized and stitched together as a unit, so the pair keeps a symmetric via fence.

7.2 Adding Vias on the Route Border

Add Stitching Vias to Route Border fences vias just inside the perimeter of the board's route border, offsetting them inward by a little more than the via pad diameter so the pads sit cleanly inside the boundary. This creates a continuous guard ring of ground vias around the routing area.

7.3 Adding Vias in Pads

Add Vias to Pad fills selected pads with a via array — useful for via-in-pad thermal and ground stitching. Select the pins or pads in Xpedition, choose the via and span, then run the action. The tool arrays vias inside each pad, honoring the span, the Try All Spans option, and the Max Density option. Round and rectangular pads are both handled.

8Filling Planes, Shapes, Obstructs, and Polygons

The center group fills copper shapes with vias — plane shapes, conductive pours, obstructs, polygons, user-layer shapes, and a selected route border. You choose whether to ring the shape with one or more loops of vias, flood its interior on a grid, or both, and then run the operation with the group's GO button. Set the Select Net for Vias field (Section 4) to the net you want these vias to carry before running.

8.1 Loops Around a Shape

8.2 Loops Around a Cutout

A shape may have an interior cutout (a cavity). The cutout options ring that inner boundary instead of the outer edge.

8.3 Flood-Filling Interiors

9Managing Via Properties

The tool can tag the vias it places with a named property. That tag lets you come back later and select, or delete, an entire group of vias at once — for example, every via that was placed to shield a particular set of RF traces. The list of property names is stored in a text file in the design's Config folder, so it persists between sessions. Three names are always available: SHIELDS, RF_TRACES, and DIFF_PAIR_TRACES.

10Add Trace Features

The lower-left group adds two trace-related features that often accompany ground stitching on RF and high-speed nets.

11Window Controls and Status

12Typical Workflows

12.1 Stitch a Ground Via Fence Along an RF Trace

1. In Xpedition, select the trace you want to fence.
2. In the tool, confirm the net was acquired and the trace width filled in.
3. Enter your operating frequency and dielectric constant in the Spacing Calculator.
4. Confirm the via to place, its hole and pad sizes, and the layer span.
5. Review the lengthwise and crosswise separations; adjust if needed.
6. Run Add Stitching Vias to Trace.

12.2 Flood a Plane with Vias

1. Set Select Net for Vias to the plane's net (usually ground).
2. Choose the via and the layer span.
3. Turn on Fill Shape Interior with Vias and set the grid spacing (and an offset if you need to align the grid).
4. Optionally turn on Stagger Interior Vias for a staggered pattern.
5. Press the group's GO button.

12.3 Ring a Pour and Remove It Later

1. Choose or create a property in the Via Property list, and turn on Add Property to New Vias so the ring is tagged.
2. Turn on Place Vias in a Loop around shape perimeter and choose Inside Shape or Outside Shape.
3. Press GO to place the loop.
4. To remove that ring later, select its property and use Select Vias with Property or Delete Vias with Property.

13Tips & Troubleshooting

• “There is no net selected”: select a trace in Xpedition before acquiring a net or adding stitching vias to a trace.
• “No Config directory found”: the design must have a Config folder beside the PCB file. The tool stores its via property list there and cannot start without it.
• Vias not appearing where expected: check that the chosen layer span actually includes the layers you are working on, and remember that with design rule checking on, vias that would violate clearances are quietly suppressed.
• Spacing looks wrong: verify the units, frequency, dielectric constant, and the trace-to-plane gap. The recommended spacings are derived directly from these values.
• A large design is slow to open: when the design contains very large numbers of vias, the tool samples them while scanning for existing properties; the progress bar shows how far along it is.
• Solder mask clearance reports an inner-layer trace: the clearance feature works on surface traces only. Deselect inner-layer traces and try again.