Auto-Interactive Routing to Overcome Obstacles and Other Polygons

Created: June 17, 2018
Updated: December 16, 2020

Image of 3D PCB routing in Auto-Interactive Routing

There’s no doubt about it, routing traces on a printed circuit board by hand can be a lot of fun. It’s an engaging challenge to make the routing as neat, tight, and correct as possible to give you the shortest routes with the best signal integrity. Once you are done you can take a lot of pride in knowing that your measured lines are perfect, you differential pairs are spot on, and everything looks great. The only problem is that level of manual precision takes a lot of time.

There are a lot of routing aids in modern PCB design software that can help you to shorten your routing time. You can find everything now from full-blown batch auto-routers to trace clean-up tools. One application that has become real handy is the auto-interactive router which allows you to direct the direction of the trace routing yourself with the speed of an auto-router. Altium Designer has one of the best auto-interactive routers available with their Active Route technology, and it can do more than help when it comes to routing around obstacles.

Manual Interactive Routing

Since printed circuit boards were first created the PCB designer has manually routed traces, first with tape on mylar and now using advanced PCB design software and its rules oriented designing. As trace routing has become more complex over time, PCB designers increasingly need automated help with routing in order to get around obstacles in less time.

Altium Designer’s PCB editor has some tools that can help with this as we will demonstrate. For a simple example, we’ve added a fill to an unrouted area of our PCB design as you can see below.

AD18 screenshot of nets to be routed in Auto-Interactive Routing

This is the area of our unrouted PCB that we will be working with

PCB designers are well versed in manually routing traces around obstacles, it just takes a little time to maneuver the trace where you want it to go. To route the four vertical nets on the right side in the picture above you would typically pick each one up individually and then “drive” it around the fill by clicking in each vertex.

Altium has helped the designer in this instance with some automation in the form of a routing engine. In the picture below you can see where the trace was pulled down and it automatically “hugged” around the obstacle for the shortest path. This frees the designer up from having to manually drive around each fill, pad, or any other obstacle that is in the way.

AD18 screenshot of manual interactive routing in Auto-Interactive Routing

“Hugging” functionality in your interactive routing will help to avoid obstacles

In the picture above you can see the segment where we simply pulled the trace down to where the green cross is, and our interactive router automatically hugged the obstacle and obediently routed around it. To accomplish this there are some settings that Altium Designer provides for the interactive router. You will find these settings by going to the “Tools” pulldown menu and selecting “Preferences”, then click on “Interactive Routing” in the PCB Editor category.

AD18 screenshot of routing preferences in Auto-Interactive Routing

The setups for Altium Designer’s interactive routing

You can see the different settings in the above picture that are provided for you. These settings are designed to make your job a lot easier when routing traces by hand. The only problem is that they only help with the manual routing of a single trace. To help with routing multiple traces at once we are going to take a look next at the auto-interactive routing capabilities in Altium Designer’s Active Route.

Auto Interactive Routing with Active Route

Active Route gives us the ability to direct the path that we want our nets to be auto-routed. To use it first open up the “PCB ActiveRoute” panel. Next, you will want to select the group of nets that you want to route. In our case, we selected the group of four vertical nets on the right side by holding the ALT key down while holding the left mouse button down and dragging the cursor from right to left over a portion of those four nets.

In Altium Designer, dragging from left to right will only select items that your select box completely encapsulates. To select items that the select box only touches you must drag the box from right to left.

Now that the four nets are selected we can start working with the router. Since our Active Route panel is already open, simply click on the “Route Guide” button. You will see your nets bunched together with a target for the cursor as shown in the picture below.

AD18 screenshot of setups for Auto-Interactive Routing

Setting up Active Route for our auto-interactive routing

Now you will digitize the path, or “river”, that you want your routing to follow. Just as if you were manually routing a single line, click in the vertices that you want for the route path. This path doesn’t have to be all the way from one end of the routing to the other, you can just specify a short distance to direct your trace routing around an obstacle as shown in the picture below.

At any point, you can use a backspace to back up what you are drawing in case you decide to change directions. You also have the ability to use the up and down arrows to increase or decrease the trace width of the path. This will adjust the amount of space needed for your group of traces that you are routing.

AD18 screenshot of guide path in Auto-Interactive Routing

Specifying the guide path that Active Route will use for routing

When you have finished drawing your path, right-click the mouse and you will see your path with the selected guides emerging on either end of the path as shown above. At this point, you are ready to route. Click on the “ActiveRoute” button in the Active Route panel, or use the keystroke combination of “Shift+A”. Altium Designer will pause for a moment and then complete the routing as shown in the picture below.

AD18 screenshot of completed routes in Auto-Interactive Routing

The completed route in Altium using Active Route

Active Route will route the entire net as far as it can go, even past the path that you have designated. It will also route un-routed portions of a net between two routed portions of the same net. This makes it an ideal tool for finishing up routing after you’ve already started work on it.

The Advantages of Altium Designer’s Active Route

One of the big advantages of Active Route is that it is all part of Altium Designer’s unified design environment. This means that there aren’t any complicated translations or transfer of data from one tool to another. Instead, you just select the nets that you want Active Route to work on and press the “go” button.

Active Route is not a traditional auto-router, instead, it is a guided interactive router that gives you high-quality routing of a set of selected nets. Yes, there are some setups that you can work within Active Route if you choose too. These will allow you to specify rules for which layers to work with, enabling a post-routing glossing pass, configuring how far Active Route is allowed to meander, and enabling pin swapping.

Active Route will also support matched net lengths as well as differential pairs. For the most part though, Active Route will use the standard design rules that you have already set up for your layout. For a PCB editor tool, it really is as simple to use as we have described here.

The key to your success with Active Route is to get into the habit of using it as part of your regular routing tools and not treating it as a complicated auto-router. The traditional thinking with a batch auto-router is to spend time setting up the design so as to make the auto-router as successful as possible. With Active Route this is not necessary. Instead, you will see the best results by putting it to use for common routing activities that would normally take you a long time by hand.

If you aren’t already using Active Route, give it a try. I’m betting that you are going to like the results that you get. Altium Designer has a lot of useful functionality built into its PCB design software to help you with every aspect of your design. Active Route is another one of those features designed to make you more productive by automating the work that you used to spend a lot of time on doing manually.

Would you like to find out more about how Altium can help you with the routing of your next PCB design? Talk to an expert at Altium.

Related Resources

Related Technical Documentation

Back to Home
Thank you, you are now subscribed to updates.