Shapester User Guide






Shapester v1.04 — User Guide | ExactCAD


Home ›
Help Files ›
Shapester

Shapester v1.04 — User Guide

1Introduction

Shapester is a productivity add-on tool for Xpedition PCB Design software (Siemens EDA / Mentor Graphics). It creates and modifies the shape of specific objects in your PCB design by using the shapes of existing objects — combining them, adding to them, or subtracting from them.

It does this in a very ‘organic’ way — the shapes stretch and flow between existing shapes rather than follow highly structured geometric forms.

Whether you need to build a plane shape that hugs a cluster of pads, create a solder mask clearance over a region, trim a plane back to the route border, or add chamfered or rounded corners to any shape, Shapester automates tasks that would otherwise require many manual steps inside Xpedition.

This guide covers every function in every window of Shapester and is written for users who have never used the application before.

2Requirements and Setup

  • Xpedition PCB Design must be open with a design document loaded before launching Shapester.
  • A valid ExactCAD license must be installed. Use the ExactCAD Licensing tool to apply your license code.
  • The setup file setup_shapester.txt must be present in the same folder as Shapester.exe. Shapester cannot start without it.
Note: Shapester connects to the currently open Xpedition session on startup. If no session is found, a message will appear and the application will close.

3Window Overview

The Main Window (title bar: Shapester v1.04) is divided into two distinct regions.

Upper region — always visible regardless of which tab is active. Contains the Copy to Other Layers controls, the Selection Info box, the Shape Creation Parameters section (Hug Pads slider, Oversize Amount, Fix/Lock options), the Corners section, and the Selection controls. Dark-red dividing lines run across the form to visually separate these groups.

Lower region — a tab control with three tabs:

  • Make Shapes — the primary tab with the most commonly used shape-creation functions: plane shapes, plane obstructs, solder mask clearances, and more.
  • Make More — additional object creation functions: route border, board-outline solder mask, conductive shapes from polygons, and perimeter plane loops.
  • Modify Shapes — tools for modifying existing shapes: round or chamfer corners, trim planes, convert between plane types, and manage pin thermal ties.

A Status label and green Progress bar run along the very bottom of the window. An EXIT button sits in the lower-right corner. The Undo button (a large dark-red X) is in the upper-right corner of the tab area.

4Upper Region Controls

These controls are always visible regardless of which tab is active below.

4.1 Copy to Other Layers

This area lets you copy selected PCB objects from one layer to one or more other layers in a single operation.

Control Purpose & Behavior
Selection Info Box The large text box at the top of the window. After pressing Copy Selected Objects, it displays a summary of what is currently selected in Xpedition — listed by object type and layer (for example, “2 Plane Shapes on layer 3”). The box automatically resizes vertically as content grows or shrinks, and all controls below it shift accordingly.
Copy Selected Objects(blue button) Reads the objects currently selected in Xpedition and populates the Selection Info Box with a summary. Press this first to capture your selection before copying.
Paste Objects(green button) Copies all captured objects to the layers entered in the Destination Layers field. A warning dialog appears before proceeding because DRC is disabled during the operation. Click Yes to continue or No to cancel.
Destination Layers(text field) Type the layer numbers you want to copy to. Use numbers, commas, spaces, and dashes in any combination. For example, 2-6, 9 11 copies to layers 2, 3, 4, 5, 6, 9, and 11. Invalid characters trigger an error message. Hover over this field to see a tooltip with additional examples.
Keep on Top(checkbox) Keeps the Shapester window above all other windows so it stays accessible while you work in Xpedition. Checked by default. Uncheck if you need another window in front of Shapester.
Delete Zero Width Traces(checkbox) When activated, scans every trace in the design and deletes any with a width under 1 mil. Reports the count in a message box. Useful for eliminating degenerate trace objects that generate false DRC violations.
Warning: Copying shapes with DRC on can produce false violations, so Shapester disables DRC for these copy operations. Always run batch DRC in Xpedition afterwards to check for genuine errors.

4.2 Shape Creation Parameters

These controls determine how new shapes are built. They remain visible at all times so you can adjust them without switching tabs.

Control Purpose & Behavior
Hug Pads Slider(track bar) Labeled Hug Pads on the left end and Stretch Between Pads on the right. Controls how tightly the created shape follows the source objects. Sliding left makes the shape wrap closely around each individual pad. Sliding right makes it stretch loosely across the space between pads. Click anywhere along the track to jump to that position. If shape creation fails because objects are too far apart, try moving the slider to the right.
Oversize Amount(text field) Enter a value to expand the resulting shape beyond the edges of the source objects. The label to the right shows the current design units (mils, inches, mm, or microns). Defaults to 5 on startup. A value of zero produces a shape that exactly matches the source geometry.
Fix Created Objects(checkbox) When checked, newly created shapes receive the Fix attribute, protecting them from being accidentally moved by the router or a manual drag.
Lock Created Objects(checkbox) When checked, newly created shapes are locked against all editing. Fix and Lock are mutually exclusive — checking one automatically unchecks the other.

4.3 Corners

These radio buttons determine the corner style for all shapes created by Shapester. Round is selected by default on startup.

Option Purpose & Behavior
Square(radio button) Created shapes will have sharp 90-degree corners.
Round(radio button) Created shapes will have smooth rounded corners. This is the default.
Chamfered(radio button) Created shapes will have flat diagonal (chamfered) corners.
Mixed Square / Round(radio button) Outside corners are square; inside corners are rounded. This is particularly useful when connecting a belly pad to surrounding ground pins — the outside corners stay neat and square while the inside curves are smooth.
Round Again(checkbox) Only applies in Mixed Square / Round mode. When checked, the outside corners are also rounded, producing an overall smoother result.
Chamfer Size(text field) Sets the chamfer distance or radius size, in design units, that is applied to corners when shapes are created in Chamfered or Mixed mode. This is a separate setting from the Chamfer / Radius Size field on the Modify Shapes tab, which is used for editing corners on existing shapes.

4.4 Selection

Control Purpose & Behavior
Keep Selection(checkbox) Checked by default. When active, pressing Undo automatically restores the previous selection set so you do not have to reselect objects before trying again with different parameters.
Reselect(blue button) Restores the last selection set that was used as source objects. Useful if you accidentally deselected your objects while adjusting parameters.
Enable Plane Selection(checkbox) When checked, existing plane shapes can be included in source selections for shape creation. When planes are included as source objects, they are incorporated into the new shape and the originals are deleted. Leave unchecked to prevent accidentally picking up plane shapes.

4.5 Undo, Status Bar, and Exit

Control Purpose & Behavior
Undo(large dark-red X button) Sends an Undo command to Xpedition, rolling back the last shape creation or modification. If Keep Selection is enabled, the prior selection set is also restored. If Bury Pins was active during the last operation, the buried thermal override is removed as well.
Status label Displays real-time messages at the bottom of the window as operations run, for example “Working on Make Plane Shape . . .” or “Make Plane Shape is done.”
Progress bar Green bar at the very bottom of the window. Fills left to right during longer operations to indicate how much work remains.
EXIT(dark-red button) Closes the Shapester application. Your PCB design in Xpedition is not affected.

5Make Shapes Tab

This is the primary tab and contains the most frequently used shape-creation functions. Select your source objects in Xpedition first, set the parameters in the upper region, then press the relevant button here.

5.1 Tab-Level Options

These controls appear at the top of the Make Shapes tab and affect the functions below them.

Control Purpose & Behavior
Use Destination Layers(checkbox) When checked, shape creation functions place the resulting object on every layer listed in the Destination Layers field rather than only on the currently active routing layer.
Make Plane Shapes Trace Keepouts(checkbox) When checked, all plane shapes created on this tab will also block traces from being routed through them.
Bury Pins(checkbox) When checked, selected SMD pins will have a “buried” thermal override applied, so they flood directly into the plane with no thermal relief spokes.
Select Net(dropdown) Populated with all net names from the design. Select a net here before using Fill Empty Spaces with Plane or Make Plane Shape on NET Pins.
Clearance / Oversize amt(text field) Sets the clearance or oversize distance used by the plane obstruct functions, the Fill Empty Spaces function, and conductive shape creation. Defaults to 15. Enter a value in the current design units.

5.2 Make Plane Shape

Creates a plane shape that encloses all selected source objects. Source objects can be pin pads, via pads, traces, plane shapes, or conductive areas. The plane is automatically assigned to the net of the first SMD pin found in the selection (or the first via, plane, or conductive area if no SMD pin is present). The new shape is highlighted in Xpedition after creation.

This function is affected by the Hug Pads Slider, Oversize Amount, Corner Mode, Bury Pins, Make Plane Shapes Trace Keepouts, Use Destination Layers, and Fix / Lock Created Objects settings.

Note: If this function fails, try moving the Hug Pads Slider farther to the right, reducing the Oversize Amount, or selecting fewer objects that are closer together. If no valid net is found in the selection, a message will appear.

5.3 Make Plane Obstruct

Creates a plane obstruct — a copper pour keep-out region — that encloses the selected source objects. Use this when specific objects need a plane clearance larger than what the design rule already specifies. Set the Clearance / Oversize amt to the desired clearance distance, select your objects, then press.

5.4 Make Plane Obstruct on Adjacent Layers Under SMT Pads

Creates a plane obstruct on the inner layer directly adjacent to each surface layer, positioned beneath the selected SMT pads. This prevents copper planes on inner layers from appearing directly below SMT pad locations — a common requirement for high-frequency or thermal designs. Select the SMT pins, set the Clearance / Oversize amt if a larger-than-pad clearance is needed, then press.

Option Purpose & Behavior
Process pads individually(checkbox) When checked, each pad gets its own individual obstruct shape. Use this when selected pads are spread far apart and it would be wrong to combine them all into a single shape.

5.5 Make Solder Mask Clearance

Creates a solder mask clearance shape on the solder mask layer corresponding to the currently active routing layer. The shape covers the selected source objects, expanded by the Oversize Amount. This shape is used as a cutout in a larger solder mask shape to expose bare copper in a specific area of the board.

Tip: The active routing layer in Xpedition must be set to the top or bottom surface layer before pressing. If an inner layer is active, a message will appear asking you to switch to a surface layer first.

5.6 Make Solder Mask Clearance from Contour

Creates a solder mask clearance shape from the outline of a selected contour, oversized by the Oversize Amount. Use the Top and Bottom checkboxes to specify which solder mask layer or layers receive the clearance.

Option Purpose & Behavior
Top(checkbox) Creates the clearance on the top solder mask layer.
Bottom(checkbox) Creates the clearance on the bottom solder mask layer.

5.7 Make Plane Shape on a Component’s NET Pins

Select the components you want to process in Xpedition first, then choose the target net in the Select Net dropdown and press. Shapester will find all pins of that net on the selected components and create a plane shape for each group. To run on all components in the design, select all components in Xpedition before pressing.

5.8 Fill Empty Spaces with Plane

Enters a click-mode. After pressing, move your cursor into the Xpedition window and click anywhere inside an open area on the active routing layer. Shapester calculates all available empty space in that region and floods it with a plane shape assigned to the net selected in the Select Net dropdown. The shape is automatically trimmed to the route border and avoids existing copper. The Clearance / Oversize amt value sets the clearance maintained from neighboring copper objects.

Note: Select a net in the Select Net dropdown before pressing. If no net is selected, a warning message will appear.

6Make More Tab

This tab contains additional board-level and polygon-based shape creation functions.

Function Purpose & Behavior
Create Route Border by Offsetting Board Outline Creates a new route border by shrinking the board outline inward by a user-specified distance. When pressed, a dialog asks for the offset distance in the current design units. The resulting route border is placed inside the board outline by that amount.
Full Layer Solder Mask Clearance Opens the Full Layer Solder Mask Clearance dialog. See Section 8 for full details. This function automates the creation of a solder mask clearance covering an entire board surface layer, with holes punched around every component pad group on that layer.
Add Solder Mask Clearance to Board Outline Adds a solder mask clearance band running along the board edge. A dialog asks for the band width, measured inward from the board edge, in design units. The clearance shape is created on both the top and bottom solder mask layers.
Delete Solder Mask Clearance from Board Outline Removes the solder mask clearance shapes previously created by the Add Solder Mask Clearance to Board Outline function. Only shapes that were tagged internally by that function are removed — other solder mask shapes in the design are not affected.
Add Solder Mask Clearance to Text Creates solder mask clearance shapes from the bounding boxes of selected text objects (conductor layer or fabrication layer texts). Select the text in Xpedition, then press. The resulting shapes expose the copper area beneath the text lettering.
Make Conductive Shape from Pin and Polygon Creates a conductive area (copper fill) within the boundary of a user-drawn polygon. Select exactly one pin and one closed polygon on a user layer — the pin origin must be inside the polygon. Shapester fills the polygon with copper of the pin’s net and automatically clears away shapes of all other nets using the Clearance / Oversize amt value as the spacing.
Make Plane Shape from Pin and Polygon Similar to Make Conductive Shape from Pin and Polygon, but creates a plane shape instead. The polygon’s outline becomes the boundary of the new plane, assigned to the pin’s net.
Make Perimeter Loop Plane Shape Creates a ring-shaped plane around the perimeter of the route border. The net is taken from the Select Net dropdown on the Make Shapes tab. The ring’s inner edge is offset inward from the route border by the Clearance / Oversize amt value; the outer edge follows the route border itself.
Note: For Make Conductive Shape from Pin and Polygon and Make Plane Shape from Pin and Polygon, the polygon must be a closed loop object and the selected pin’s origin must lie inside the polygon boundary. Error messages will appear if these conditions are not met.

7Modify Shapes Tab

This tab provides interactive tools for modifying existing shapes in the PCB design.

7.1 Round Corner

Converts a sharp corner vertex in an existing shape to a smooth rounded arc. After pressing, move your cursor into the Xpedition window. A red diamond snap marker appears near each vertex as you hover over the shape. Click near the vertex you want to round — it will be replaced with an arc of the radius set in the Chamfer / Radius Size field.

Option Purpose & Behavior
Chamfer / Radius Size(text field) Sets the radius for Round Corner or the flat-cut distance for Chamfer Corner, in the current design units. Defaults to 20.
Chamfer / Round Entire Shape(checkbox) When checked, clicking anywhere on a shape applies the operation to all vertices of that shape simultaneously rather than just the nearest one. Vertices whose adjacent line segments are too short to accommodate the radius or chamfer are skipped automatically.
Tip: Move your cursor slowly over the shape — the red diamond snap marker snaps to the nearest vertex and shows you exactly which corner will be affected before you click.

7.2 Chamfer Corner

Identical in operation to Round Corner, but replaces the sharp vertex with a flat diagonal cut rather than a curved arc. Hover near the vertex to see the red diamond snap marker, then click. The cut distance is set in the Chamfer / Radius Size field. The Chamfer / Round Entire Shape checkbox applies here as well.

7.3 Trim Planes to Route Border

Trims the selected plane shapes so no portion of them extends beyond the route border. Net assignment, hatch pattern, and all other plane properties are preserved. Select one or more plane shapes in Xpedition, then press.

7.4 Trim Plane with Another Plane

Interactively trims one plane shape using the outline of another as the cutting tool.

  1. Press the button. A dialog asks you to select the plane to be trimmed. Click it in Xpedition and click OK.
  2. A second dialog asks you to select the plane to use as the trim tool. Click it and click OK.
  3. The trim tool’s outline is expanded by the Clearance / Oversize amt value from the Make Shapes tab, and a cutout matching that expanded shape is placed in the first plane.
Note: The Clearance / Oversize amt field on the Make Shapes tab must contain a numeric value before using this function.

7.5 Convert Conductive Area to Plane Shape, or Shape to Area

Converts selected objects between their two type variants without altering their shape or net assignment. Selected plane shapes become conductive areas; selected conductive areas become plane shapes. Select the object or objects in Xpedition, then press.

7.6 Set Diameter of Userlayer Circle

Changes the diameter of all selected circle objects on user layers. Select the circles in Xpedition, press this button, then enter the desired diameter in the dialog that appears. All selected circles are redrawn at the new size.

7.7 Bury Pins / Thermal Tie Pins

Function Purpose & Behavior
Bury Pins(blue button) Applies a “buried” thermal override to all selected pins, flooding them directly into their associated copper plane with no thermal relief spokes. Select the pins in Xpedition, then press.
Thermal Tie Pins(blue button) Removes the buried thermal override from all selected pins, restoring them to the default thermal relief behavior defined by the design rules. Select the pins, then press.

8Full Layer Solder Mask Clearance Dialog

This dialog opens when you press the Full Layer Solder Mask Clearance button on the Make More tab. It automates the creation of a complete solder mask clearance covering an entire board surface layer, with cutout holes placed precisely around every component pad group on that layer.

Use this function when a board requires bare copper across an entire surface — for example, a ground plane exposed for heat dissipation — except at the component pad locations.

Control Purpose & Behavior
Select Layer(dropdown) Choose Top or Bottom to specify which surface layer receives the solder mask clearance.
GO(button) Starts the operation. Shapester scans all components on the selected layer, groups pads that are spatially close together so that adjacent pads share a single hole in the solder mask, then creates the large board-covering solder mask shape with cutouts punched around each group. This process can take several minutes on large or dense boards.
Status label Displays real-time progress messages such as “Collecting pins . . .”, “Grouping pins . . .”, and “Done with Auto Full Layer SM clearance.”
Progress bar Shows how far along the current step is.
Close(button) Closes this dialog and returns to the Main Window.
Tip: Before opening this dialog, set the Hug Pads Slider all the way to the right and the Oversize Amount to at least 10 mils (0.25 mm) in the Main Window. These settings determine how much solder mask coverage is left around each pad group. If these settings do not produce the desired results, delete the solder mask shape, adjust the settings, then try again.

9Typical Workflows

9.1 Creating a Plane Shape Around Multiple Pads

  1. In Xpedition, select the pads and/or vias you want the plane shape to enclose.
  2. In Shapester, set the Oversize Amount to your desired clearance above pad edges.
  3. Adjust the Hug Pads Slider — start toward the right for a looser, better-connected shape.
  4. Choose a Corner Mode (Round is the most common choice for power planes).
  5. Press Make Plane Shape on the Make Shapes tab.
  6. If the result is not right, press Undo, adjust the settings, and try again.

9.2 Copying a Shape to Multiple Layers

  1. In Xpedition, select the shape or shapes you want to copy.
  2. Press the blue Copy Selected Objects button in Shapester.
  3. In the Destination Layers field, type the target layers (for example, 2-5, 8).
  4. Press the green Paste Objects button.
  5. Acknowledge the DRC warning and click Yes to proceed.

9.3 Adding Rounded Corners to an Existing Shape

  1. Switch to the Modify Shapes tab.
  2. Enter the desired radius in the Chamfer / Radius Size field.
  3. Press Round Corner, then move your cursor into the Xpedition window.
  4. Hover near the corner vertex — the red diamond snap marker will appear, indicating which vertex will be rounded.
  5. Click near the vertex to apply the rounded arc.
  6. To round all corners in the shape at once, check Chamfer / Round Entire Shape before clicking anywhere on the shape.

9.4 Full Layer Solder Mask Clearance

  1. In the Main Window, set Oversize Amount to at least 10 mils (0.25 mm).
  2. Move the Hug Pads Slider all the way to the right.
  3. Press Full Layer Solder Mask Clearance on the Make More tab.
  4. In the dialog, select Top or Bottom.
  5. Press GO and wait. Large boards may take several minutes — watch the progress bar.

10Tips & Troubleshooting

  • Shape creation fails: Try moving the Hug Pads Slider farther to the right. The selected objects may be too far apart for the current slider value to bridge between them.
  • DRC errors after pasting: The Copy to Other Layers function disables DRC during execution. Always run batch DRC in Xpedition afterwards to check for genuine violations.
  • Wrong net assigned to a created plane: The net is taken from the first SMD pin found in the selection. Verify the correct pins are selected before pressing Make Plane Shape.
  • Undo does not restore the selection: Make sure Keep Selection is checked if you want your selection preserved after undoing.
  • Full Layer SM takes a very long time: Large or dense boards can take several minutes. Watch the progress bar and do not interact with Xpedition while the operation runs.
  • Cannot see the Shapester window: Make sure Keep on Top is checked. Click the Shapester entry in the Windows taskbar to bring it to the foreground.
  • License error on startup: Use the ExactCAD Licensing tool to apply your license. The file is stored at %LocalAppData%\ExactCAD\Exactcad_License.txt.
  • Setup file missing error: Ensure setup_shapester.txt is in the same folder as Shapester.exe. Shapester cannot start without this file.
  • No Xpedition session found: Xpedition must be open with a design loaded before launching Shapester.
  • Trim Plane with Another Plane does not work: Make sure the Clearance / Oversize amt field on the Make Shapes tab contains a numeric value before using this function.