Skip to main content

What's New in OrCAD X 24.1 (Webinar Recap)

Key Takeaways

  • Live BOM forecasting and Workspace updates make project management easier within OrCAD X Capture.

  • New features in OrCAD X Presto include docked Constraint Manager rules, a new Footprint Generator, and more.

  • The Analysis Workflows give designers a powerful tool to analyze signal integrity through impedance and coupling analyses.

View of OrCAD X Capture 24.1 launch window.

What’s new in OrCAD X 24.1 is several features to expedite design analysis.

OrCAD X sees its first major update with the release of version 24.1, which introduces a host of new features that give design teams greater analysis of their design at the schematic and board levels. What’s new in OrCAD X 24.1? Multiple new or expanded features help accelerate project designs with a focus on analysis and a simplified UI that keeps designers focused on the board.

A Summary of What’s New in OrCAD X 24.1

OrCAD X Capture

OrCAD X Presto

  • Live BOM Forecasting
  • Workspace file management
  • PSpice measure command
  • Constraint panel
  • Footprint Generator
  • Place and Move command updates
  • New visibility toggles (Shadow and Custom Color)
  • Workspace Analysis (Impedance and Coupling)
  • Cut Trace command
  • New Shape engine

What’s New in OrCAD X 24.1 for OrCAD X Capture

Live BOM Forecasting

View of Live Bom forecasting feature.

Live BOM forecasting helps users anticipate market changes.

In addition to the current procurement analysis capabilities of Live BOM, users can now project lead times, availability, cost, and inventory with the powerful Sourcengine. By staying ahead of supply-demand crunches, procurement teams can optimize budgets and purchasing windows to prevent avoidable disruptions to design turnaround time. Designers can get a more granular view of week-to-week supply forecasts by hovering the mouse pointer over the generated line graphs, including a summary of the delta (in weeks, dollars, inventory, etc.) to capture the difference between current and future procurements succinctly. The right-hand side of Live BOM provides a convenient summary of the forecast highs, lows, and averages for the various attributes.

Workspace File Management and UI Improvements

A view of files copied from File Explorer to OrCAD X Capture File Manager.

OrCAD X Capture 24.1 users can quickly add files to their projects.

Users can drag and drop project files and folders directly into Workspaces folders from local directories. The “Add New” button above the folder hierarchy in the Workspace view opens a File Explorer window for easy browsing. The Workspace Configuration UI now shows information regarding file storage residency and whether the file residency is internal or external to the organization:

  • Internal file locations are only accessible to some or all OrCAD X users with the same company domain.

  • External file locations extend Workspace access to users outside of the company domain.

Creating custom Workspaces is straightforward: navigate to the top right of the Workspace Configuration dialog and select New Workspace. Users then name the Workspace, indicate its server residency, assign the default access role (Administrator, Designer/Librarian, Designer, Librarian, or Viewer), and select between default Workspace access to all members of the company domain or through invites (users can also provide external access by checking the final option). For global company domain access, users will see a “*@[domain_name]” in the bottom half of the Workspace Configuration dialog that indicates all domain users' default level of access. However, those with Administrator privileges can override the default access level for specific users by entering their email addresses and selecting a new role from the populated list. Adding external users follows the same workflow process: enter the email address, then select the user role from the populated list.

View of Workspaces in Workspace Configuration

The new Workspace Configuration window displays data residency.

PSpice Enhancements

24.1 users can integrate .MEAS (measure) commands into their PSpice commands:

  1. In a .txt file, users specify .MEAS commands (with appropriate parameterization), then save the file with a new extension: .inc (include). 

  2. Open Simulation Settings in OrCAD X 24.1, then select Configuration Files in the leftmost dialog box. 

  3. Change the category to “Include”, then browse to the .inc file location. 

  4. Click “Add to Design” and finalize the PSpice settings with “OK”. 

  5. Run the simulation, and navigate to the PSpice simulation file location (in the PSpice window, select “File” > “Open File Location” from the top navbar.

  6. Locate a .txt file extension with a name ending in “ _measure”. The measurements described in the .inc file are in this file.

OrCAD X 24.1 Layout Improvements

Constraint Panel Update

View of OrCAD X Presto canvas emphasizing Constraint Panel.

The Constraint Panel facilitates quick editing of the design rules.

New in 24.1: users no longer have to navigate to Constraint Manager to view or change their constraint rules – they are conveniently located within the Constraint Panel in the Design Canvas to keep the focus on the layout. Users create a rule set and apply those rules to nets with similar requirements (e.g., power, high-speed, differential pairs, etc.) Like in the Constraint Manager, rules have four categories – Electrical, Physical, Spacing, and SameNetSpacing – with a toggle option for basic and advanced rules:

  • Electrical

    • Basic: Ratsnest scheduling (topology), etch length, stub length, total etch length, max via count

    • Advanced: Differential pair (max uncoupled length, static/dynamic phase control)*, delay (pin pairs, absolute min/max delay, relative min/max delay), return path (reference net, reference layers, max unreferenced length), single-ended trace impedance

  • Physical 

    • Basic: Single-ended (neck width, neck length, max width), differential pair (neck gap, neck width, trace gap, trace width), via structure (pad/hole shape, pad/hole size, solder mask/paste mask expansion)

    • Advanced: Individual layer filter, single-ended (min width, blind/buried via stagger, pad-to-pad connections, layer etch, T-connections) differential pair (max uncoupled length, static/dynamic phase control)*

  • Spacing/SameNetSpacing

    • Basic: Spacing (pad-pad, pad-line, pad-shape, line-line, line-shape, shape-shape)

    • Advanced: Spacing (via pad-via pad, via pad-line, via pad-shape, via pad-pin pad, pin pad-line, pin pad-shape, pin pad-pin pad), pad spacing (thru pin-thru pin, thru pin-SMD pin, thru pin-shape, thru pin-line, thru pin-BB via, thru pin-microvia, thru pin-thru via), hole spacing (hole-hole, hole-line, hole-pin pad, hole-via pad, hole-shape), hole type spacing (thru via hole-thru via hole, thru via hole-BB via hole, thru via hole-micro via hole, thru via hole-pin hole)

*: These rules are found in two locations for optimal user preference.

The Constraint Manager isavailable for more detailed rule creation and is now accessible directly from the Constraint Panel.

New Footprint Generator

View of Footprint Generator highlighting a standard BGA package.

The Footprint Generator makes creating IPC-compliant footprints easy based on package geometry.

Users can launch the Footprint Generator from “File” > “New” > “Template based footprint” and generate footprints based on IPC rules. It’s quick to navigate between surface mount device (SMD) and through-hole (TH) footprints for the major package families. Clicking on a particular IPC footprint displays the model and the dimensions/parameters of the package (pin count, pitch, body length/width, etc.) A dropdown selection for assembly density producibility (IPC-A, B, or C) gives designers additional control to tighten or relax tolerance for component placement. Once all selections/parameters are final, click “Generate” in the top-left to finalize the footprint.

Generated footprints contain all necessary data/shapes/information, such as padstacks, place bound regions, and keep ins/outs alongside a 3D model. Modifying the footprint is also straightforward: users can edit directly in the canvas, or relaunch the Footprint Generator from the Source template refresh button. Updating any data in the footprint generator and regenerating the footprint replaces the old footprint.

Accelerate Designs with New Place-and-Move Commands

View of layout highlighting traces and Place and Move command window.

Users can have the Place and Move commands in the design canvas or dock them in a panel.

OrCAD X 24.1 offers designers industry-leading features and options to reduce time spent during component placement. After selecting the Move command in the Design Canvas, the Move Options will display in the docked panel. Users can also summon the options menu from its docked position to the mouse location (and toggle it back to a docked view) by pressing “X”:

  • Traces - When moving components, users can choose between Ripup and Slide. The Slide option moves the traces with the component, while Ripup reconnects them at their previous intersections. 

  • X-Y Display - Picking up a component displays the previous x-y location of the component origin and the current x-y location of the component origin (while it’s attached to the cursor). In absolute mode, the current x-y location is relative to the origin of the board. In contrast, relative mode displays the change in the x-y position from its selected initial location. With a component selected, hit “Tab” to open a dialog for precise x-y location – in absolute mode, users enter the desired position, while relative mode accepts a +/- difference from the initially selected location.

  • Move Origin - Users can change the origin of the move command from the selected component origin to an object location on the board. This option helps arrange placement relative to a large or central component. 

  • Alignment Guides - These guides keep the layout organized and aesthetically pleasing. Users can align by the component origin, place bounds, connection lines, or any combination.

  • Temporary Relative Grid - This option temporarily overrides the global design grid for a relative grid defined by a user-selected object (e.g., a pin of an SD card reader). The temporary grid makes it easy to arrange and align components locally.

New Visibility Options for Design Readability

Layout view showing mid-shadows and custom colors off.

The Shadows and Custom Colors options (pictured bottom-right) support greater visibility customization.

OrCAD X 24.1 users can locate two new visibility features in the bottom-left corner of the Design Canvas (in line with the layer view options):

  • Shadows  - Users can toggle between three settings: off (default view), mid-shadow (any selected same-net objects will appear as hatched lines of the layer and the net color), and on (only the net’s colors are visible while the rest of the design is in grayscale). 

  • Custom Colors - Designers often use a custom color to distinguish nets from their surroundings during layout (especially for same-layer objects). However, this can remove some detail when taking a “big-picture” look at the design. Users can see the layers nets traverse while maintaining the assigned custom color by toggling custom colors off.

New In-Design Analysis Workflows

View of impedance analysis results.

Analysis Workflows give layout designers a tool to check signal integrity.

By launching the Analysis Workflow (under “View” > “Panels” > “Analysis Workflow” in the top navbar), users can investigate the impedance or coupling of the design in visual and tabular formats. After setting the analysis options and running the analysis, users can view all trace segments on a color-coded scale (red = highest, blue = lowest, green = nominal) for single-ended traces and differential pairs. Sliding the top or bottom of the scale, users can see only the impedances/coupling coefficients that fall within the bracketed range (helpful in locating high/low values) and update the design in real time as the design analysis overlays on top of the layout. In the docked Simulation Table, the analysis displays sortable net characteristics depending on the analysis mode in a Summary and Detailed Table:

  • Impedance - Max/minimum impedance, length, via count, delay, inductance, capacitance, resistance

  • Coupling - Net, aggressor net, coupling coefficient, coupling coefficient length

Besides net-based analysis, users can also run directed group analysis, which uses signal drivers/receivers to measure impedance/coupling. With the directed group analysis, users can generate an additional plot that visually indicates the analysis along the trace length (in “Bar/Expanded”) or graph the segments by value/segment length independent of the trace run.

Faster Layout Design

View of Cut Traces command.

Features like Cut Traces accelerate ECO footprint changes.

  • Cut Traces - When updating footprints (e.g., component replacement due to cost/availability/lead time issues), users can use the cut trace command to remove trace segments instead of entire traces. Select the Cut Trace tool, click the starting point, and drag the cursor across the desired trace segments. After replacing the footprint, users only need to reconnect the dangling trace segments instead of rerouting the nets entirely.

  • New Shape Engine - When drawing polygons, users can cycle through three modes with “Q”: line, arc, and circle. The angle lock (“A”) toggles polygon vertices/arc constraints between freeform and standard angle settings, while “C” (only in circle mode) enables users to set an inline or outline arc.

View of Add Shape window overlaying board layout.

The Add Shape window can quickly cycle through design options.

Cadence Solutions Make PCB Layout Faster and More Intuitive

Users interested in seeing what’s new in OrCAD X 24.1 can get started today with a free trial and see the next generation of PCB layout software. Beyond the update, OrCAD X features an intelligent user interface focusing on the board design to accelerate design turnaround. Interested in learning more? See the full Cadence PCB Design and Analysis Software catalog supporting current and future electronics innovations.

Leading electronics providers rely on Cadence products to optimize power, space, and energy needs for a wide variety of market applications. To learn more about our innovative solutions, talk to our team of experts or subscribe to our YouTube channel.