Skip to main content

Managing Constraints Like a Pro in OrCAD X FAQ

Published Date
Author Cadence PCB Solutions

Here are some comprehensive answers to all the questions asked in our recent webinar. 

Constraint Manager | Constraint Files | OrCAD X Presto PCB Editor | General

    Constraint Manager

    Let’s say I have two parts in my design, U1 and U2. I have placed those parts and now want to make sure their distance will not change. Is there any maximum distance constraint I can apply between the two Parts? Within the DFA constraint, I can only see minimum distance. 

    Within the Constraint Manager in OrCAD X, there is currently only a minimum spacing constraint that you can set between two parts. However, to limit distance between U1 and U2, you could create a max delay constraint on a connection between U1 and U2. That would work like a max distance between the 2 components. 

    How can I clear or delete all constraints for design? 

    In the Constraint Manager you can select the top field for the constraints and clear the value, which will clear the constraints for everything. If you want to delete all constraints from your design and start with a clean slate, the easiest way would be to simply open up a new database and export an empty constraints file (.dcfx), then import that empty constraints file into your existing database – this way you can ensure you don’t accidentally miss any manual overrides that could have existed.

    Do region constraints automatically correct any existing routes/placement within the design? 

    Applying region constraints on existing routes/placement does not automatically correct them within your design, but it’ll flag them with a DRC. However, if you make any changes to the existing elements like moving components or sliding traces that are within the region constraints, the changes will automatically apply.

    How can we setup minimum spacing distance between two nets?

    Within the constraint manager, go to the Spacing worksheet. Under Spacing Constraint Set select All Layers. Right click on Dsn and select Create – Spacing CSet. Assign a name for your spacing rule. Then in the relevant columns such as line to line or line to via define the specific minimum spacing distance that should exist. Once you’ve defined the spacing constraints set, go to the Net – All Layers to apply the spacing constraint that you just created for both the nets.

    How can a designer see the applied constraint created for the spacing of two planes in an existing design, when performing any review? 

    Select the two planes and view the resolved spacing area in the constraint panel.

    Is there a priority ranking for rules? How do you ensure the priority of a rule between the constraint manager (electrical, physical), the parameters on the board, the DRC and the analyze and software setup parameters? 

    There is no priority of rules, but there is a hierarchy. Aside from similar rules between design for fabrication and spacing constraints there also isn't any overlap so there isn’t a need for priority.

    Is there a way to attach a region constraint to a component. So that if the component is moved, the region will move too? 

    No, you cannot add region constraints to a component.

    How do you define spacing between net groups or classes when they are routed on different layers in Z-axis? 

    Depending on the reason you can use creepage and clearance DRC rules available in higher tiers of Allegro X if the spacing is for high voltage.  If you’re looking for Z-axis spacing for high-speed then you can tell the constraint manager to check for Z-axis.

    Can you still set up delay maximum by time (ns) instead of length (mil)?

    Yes, all electrical constraints can be entered in units of length or time. You can set your preferred option by toggling the unit in the column header of the electrical worksheet within the Constraint Manager.

    When importing constraints in a design, if there are any differences, will it show us what they are? And how would I resolve those? 

    Yes, a difference report will be generated automatically and based on what the differences are, it’s up to you on how you want to resolve the conflict. 

    How would I specify backdrill information within the constraint manager?

    You can specify backdrill information from within the Properties worksheet in the Constraint Manager. Under Net, select General Properties and enter in a value for Max PTH Stub for the necessary nets.

    Constraint Files

    Can the constraints be exported as a file? If so, what file type is it? 

    Yes, constraints can be exported from within the Constraint Manager (CM) under File > Export as either a technology file (.tcfx) or a constraints file (.dcfx). The technology file will only export the rules you created, and the constraints file will export both the rule and the nets the rule it should be applied to.

    How can I import an Excel spreadsheet with rules into constraint manager?

    This functionality is only available in higher tiers of Allegro X. To import an Excel spreadsheet with rules, you would have to use the Allegro X constraint compiler.

    What information does the technology file import and export? Is it only the constraint sets and groups? Does it include which specific nets are included in those groups/which constraint sets are applied to them? 

    You have some options to specify what is exported and imported. The technology file will only export the rules you created. If you want the imported rules to be applied to specific nets, you’ll need to export and import a constraints file as it will contain the information on both the rule and the nets the rule it should be applied to.

    OrCAD X PCB Editor

    What is OrCAD X and what is OrCAD X Presto PCB Editor? 

    Cadence OrCAD X is one of our PCB design platforms that includes applications for schematic, simulation, and layout. Presto PCB Editor is the latest layout tool available within the OrCAD X platform.

    When will autorouting be released in OrCAD X Presto PCB Editor? 

    The traditional Spectra autorouter is available in OrCAD X PCB Editor - there are no plans to introduce this into OrCAD X Presto PCB Editor. X AI is the new AI based placement and route solution that is integrated into Presto PCB Editor and is currently only available to a few collaborating customers as we mature the technology. 

    Is possible to have the side panes "floating" and "attached" to cursor position and activate it with dx mouse button?

    The side panes aren’t activated by a mouse button click, however they can be undocked and moved to your desired location if you click on the pin icon within the pane. In OrCAD X 24.1 we added support for docking and recalling command panels to the cursor using the X key.

    Can you click on a line in PCB routing and see which rule(s) affect this line? 

    Yes, in the 24.1 release, we’ve introduced a docked constraint panel within OrCAD X Presto PCB Editor which will show you this information. Within OrCAD X PCB Editor, you can do this by using the Constraints Show (Cns Show) command from the toolbar and use the find filter to ensure you have either nets or clines selected before clicking on any line(s).

    General

    What is a Batch DRC? 

    Design rule checks (DRCs) are either "online" or live, meaning that you would see errors reported as you are editing in the canvas. Batch DRC is when you run a larger number of checks in a single run (hence the name batch) and will get violation results for whatever DRCs you chose to run. 

    Is OrCAD X 24.1 the latest version? 

    Yes, OrCAD X 24.1 was released on Friday, September 20, 2024. 

    Can I reuse the strokes I have been using from Allegro 22.1 to Allegro X 24.1? 

    Yes, strokes files are transferable. Simply save any strokes you’ve created in 22.1 to a specific directory of your choosing and easily open it in 24.1.

    Can you select a net in Constraint Manager (CM) by selecting nets from the schematic? Normally I set my constraints in schematic and do not change in layout anymore. 

    Yes, you can do that. There is also a new simplified integrated CM panel available within OrCAD X Presto PCB Editor 24.1 that allows you to select nets in the canvas and assign constraints sets based on the selection.

    Can you assign constraints at schematic level if you just use a blank board with stack up defined before component placement? The reason for the question is that you may have someone else doing the PCB layout. 

    Yes, you can assign constraints at the schematic level. The same constraint manager exists in OrCAD X Capture as it does on the PCB layout side allowing you to specify electrical constraints. You can access the Constraint Manager in OrCAD X Capture from the toolbar or by from the PCB > Constraint Manager menu.

    Can same net spacing constraints violation be checked as a DRC? 

    Yes, same net spacing violations will appear as DRCs. 

    Does the Electrical Constraint Set- Impedance actually adjust the width of the trace while routing or is it only for auditing? 

    This constraint can be used for both, so it’s up to you to determine if you want it to drive trace width or check for impedance instead.

    Can constraints for PCB be placed at schematic level (before any PCB development) and be locked for the rest of the design flow? 

    Yes, you can enter constraints at the schematic level, however they can’t be locked from future editing or changing.  Instead of locking you can always drive constraints from schematic to PCB. 

    I’m currently in my final year of college, does Cadence offer any courses or internships for students? 

    Yes, we do offer internships - we would suggest checking our career openings on cadence.com. Product training is offered both online and in a classroom. Online classes can be found for free through our learning management system on cadence.com. 

    When I create constraints in Cadence Design Entry, do I need to manually export constraints, then manually import the constraints into Allegro X PCB?  Or when I export from design entry, and import netlists into Allegro X PCB, does it automatically bring it in? 

    Electrical constraints will be propagated from the schematic environment to PCB layout. There are situations where constraints may not fully sync - in this situation you can export the technology file and import them into the PCB editor to resync the designs. 

    How can I import the logo of company inside the PCB layout? 

    If you have access to Cadence Online Support there is an article that covers this step by step. Here is the link.

    Why do the line width and neck width have to be the same for differential pairs? What if you needed a larger width as your default width but need a neck down width?

    If possible, when routing differential pairs, it is recommended that your line width be the same to ensure consistent impedance throughout the length of the traces to minimize degradation (loss, reflection, crosstalk). At times you may need to use neck mode to route through a tight area like a BGA, so it’s crucial that you keep the neck mode region as short as possible to avoid altering the impedance by too much.

    How can I check the definition of the Power Nets in OrCAD X Capture without going and checking all the Power Net Global and the Power Pin in the schematic?

    Unfortunately, there is not a simpler way to do this in OrCAD X Capture.

    How can I highlight a net or group with a specific color?

    Within the Visibility pane in OrCAD X Presto PCB Editor, you can click on the Nets tab and find the net or group you want to highlight. Select the net, multiple nets or the group and right click to assign a color.

    What is the difference between classes and groups?

    Classes and groups are two different ways of organizing and managing design rules for your PCB components. Classes provide broad rule application and groups allow for more granular control within or across the classes.