Blog

Tutorials, news, snippets, and other various musings about the electrical engineering industry.

Quick Tutorial: Real-Time Routing Analysis


 

Design Rule Checks are usually performed to identify and resolve any features that may be troublesome for your design, including signal quality and manufacturing issues. Performing these checks AFTER your design is completed can lead to design re-spins or re-routing specific portions of your design. Easily find route quality issues during the routing process with Real-Time Routing Analysis in OrCAD PCB Designer Professional.  This tutorial will show you how to use the user-configurable checks to find and resolve issues in your design in real-time, improving performance and optimizing your design. If you would like to follow along with this tutorial,you can download the design files here.
 

Step 1: Open your design in OrCAD PCB Designer Professional and open the Vision Manager by selecting Display --> Vision Manage from the menu.

Select Routing Vision from the drop-down menu.
 


 

Step 2: Set up the Route Vision Manager.

Set the Color for non-optimized traces by clicking on the color square and selecting the desired color or use the default settings.
Select “Dynamic Log” and “Log Current View Only”.
 

You can activate this view by selecting “View Log” in the Route Vision Manager at any time.
 


 

Step 3: Configure the Route Vision Manager. Click Configure.
 

1. Select the following options from the Route Vision Configure Window and Click Ok:

  • Parallel Gap Less Than Preferred
  • Non-Optimized Segs
  • Non-Ideal Pad Entry
     


 

2. In the Route Vision Manager, set the following values:

  • Parallel Gap Less Than Preferred: 15.00
  • Non-Optimized Segs: 50.00
     


 

Step 4: Route your design to review “Non-Optimized Segments”. Select Routeà Connect from the menu.


1. Route the connection between vias for net A4_ADC_GPIO. Right click and select Done.
 


 

2. Delete the previously routed trace by selecting the trace and clicking the “Delete” button on the toolbar.
3. Select Route  --> Connect from the menu. Under the Options tab, click “Optimize in Channel”.
4. Re-Route the connections between the vias for net A4_ADC_GPIO.
 


 

Step 5: Route your design to review “Non-Ideal Pad Entry”. Select Routeà Connect from the menu.

1. Begin to route the trace for net A1_MUX. Right click and select Done.


 

2. Select Route  -->  Slide from the toolbar. Adjust the trace until an ideal pad entry is achieved.
 


 

Step 6: Route your design to review “Parallel Gap Less Than Preferred”. Select Routeà Connect from the menu.
 

1. Begin to route the trace for net A2_MUX. Right Click and select Next.
 

2. Begin to route the trace for net A0_MUX. Right Click and select Done.


 

3. Select Route  --> Slide from the toolbar. Adjust the traces until the desired parallel gap is achieved.
 


 

OrCAD PCB Designer Professional provides real-time, visual feedback for nine common, route-quality issues. Utilizing this feature in the routing phase of your design, instead of performing a post-route design rule check of constraints, will reduce time and resources spent on design changes and re-spins. With real-time routing analysis, you can catch these potential problems during your routing process; optimizing your design and improving signal quality as you go.
 

When configuring Route Vision, OrCAD provides additional information as well as images for further clarification.