How to Simplify Your Circuit Replication with Multi-Channel Design

March 27, 2017 David Cousineau

Multi channel PCB design layout example

Circuit replication, particularly in flat designs, presents several unique challenges that can be intimidating for any designer. Use a multi-channel design to efficiently replicate circuitry and routing data to successfully overcome the common challenges associated with flat designs.

The Advantages of Multi-Channel Design

Altium Designer offers many methods for multi-channel design (i.e. repeating circuitry within a single design). The main advantage of multi-channel design is that any change to the underlying circuit need only be made once. And that change will immediately be seen in every instance.

There are many users, however, who have not worked with hierarchical designs and feel more comfortable using a flat design methodology. Or some projects may just be too simple to warrant setting the entire design as hierarchical. Whatever the case, there are a number of legitimate occasions wherein the Project is set up as flat, but circuit replication is necessary and the layout of that circuit also needs to be replicated. How can this be done?

Flat Designs Using Multiple Sheets

In the use case of a flat design using multiple sheets, you’ll find that Altium Designer will automate most of this process for you. In fact, there will be only one bit of manual intervention required by the user in the PCB document during the process.

Let’s walk through an example to see how this works. In our example below, we need to replicate the Channel 1 circuit once.

 

Channel 1 Schematic before replication

Channel 1 Schematic Requiring Replication

Step 1 - Schematic Creation Replication

We’ll start by creating the initial circuit on the first schematic sheet of a PCB project (named “Channel_1.SchDoc” here). Then add a second, empty schematic sheet (“Channel_2.SchDoc”) to the Project.

The Channel_1 circuit now needs to be copied and pasted to Channel_2. If the reference designators have already been set for the base circuit, go to the DXP menu and then to Preferences. Expand the Schematic group and select the Graphical Editing section. In the Options area, enable the “Reset Parts Designators on Paste” option.

 

Resetting parts designation in DXP Preferences

Resetting the Parts Designation On Past Settings in DXP Preferences
 

Next we’ll group-select the base circuit, copy it, and paste it to Channel_2 then make any edits necessary to the second circuit to ensure proper connectivity with the rest of the design. In this case, the “Pulse1” and “Peak1” ports have been made unique, as has the “Channel 1” text identifier.

 

 

Screenshot in PCB design software of Replicating Existing Schematic capture

Replicating Existing Schematic to Create Channel 2 Design

 

 

We can now add whatever additional sheets are necessary for the design. However, it is important that no further additions or changes be made to any of the repeated schematic sheets. Doing so may cause the Copy Room Formats feature to fail later on. For this project, a third sheet (“Connector.SchDoc”) will be added to include a connector with the design.

Since the reference designators on Channel_2 have all been reset to ?, we can run Tools/Annotate Schematics Quietly to set the designators.

Another important note has to do with multi-part components. In this example, only parts A, B, and C from the op-amp (TL074ACD) are being used, while part D is not. Make sure that when the reference designator annotation is done, unused parts from one circuit are not used in another. There needs to be consistency between each physical circuit so that the routing can match. Here, U1A, U1B, and U1C are used in Channel 1, but U1D does not get used for Channel 2. Instead, Channel 2 starts off at U2A.

Step 2 - Project Options Setup

The next step is to set the Project Options to automate the Component Class and Room generation. To do this, we’ll go to Project/Project Options and switch to the Class Generation tab.

 

 

Multichannel design screenshot of Project Options

Automating Component Class and Room Generation in Project Options

 

 

We need to ensure that the checkboxes for Component Classes and Generate Rooms are enabled for all multi-channel sheets. Any other sheets are optional. To finish up, we’ll close the Project Options dialog and save all schematic documents, as well as the Project file.

Step 3 - PCB Layout

The final step is to create and save a new PCB file, then use Design/Import Changes… to populate the board. Ensure that the ECO includes the creation of the Component Classes and Rooms. If not, recheck the Project Options setup done previously.

The PCB will then be populated with the Rooms as shown below:

 

Screenshot of PCB design populated with designated rooms

PCB Populated with Designated Rooms
 

We can then move the Channel_1 Room into the board area, then place and route it as desired. Resize the Room outline if necessary.

 

Channel 1 Board Layout in PCB design software tool

Completed Channel 1 Board Layout

 

Flat Designs Using a Single Sheet

A second multi-channel situation makes use of a much smaller circuit, copied and pasted many times within the same sheet. In this case, it would not be very efficient to create a separate sheet for each circuit, as in the previous example. As mentioned, though, this method requires a few more manual steps in order for Copy Room Formats to function correctly.

To learn how to accomplish this multi-channel situation by downloading a free white paper.

 

About the Author

David Cousineau

Dave has been an Applications Engineer for 20 years in the EDA industry. He started in 1995 at a mid-Atlantic reseller that represented PADS Software, ViewLogic, and a host of other EDA tools. He moved on to work directly for PADS Software, and stayed on as they were acquired by Innoveda and then by Mentor Graphics. He and a business partner formed a VAR of their own in 2003 (Atlantic EDA Solutions) to represent Mentor's PADS channel, and later on Cadence's OrCAD and Allegro products. Since 2008, Dave has been working directly for Altium and is based at his home office in New Jersey.

More Content by David Cousineau
Previous Article
Why Use Through-Hole Technology in PCB Design?
Why Use Through-Hole Technology in PCB Design?

When it comes to technology, we never look back, always forward. Sometimes, though, it seems that the old t...

Next Article
How the Evolution of PCB Design Has Allowed SpaceX's Visions to Take Flight
How the Evolution of PCB Design Has Allowed SpaceX's Visions to Take Flight

Today, the new frontiers of spaceflight are explored by SpaceX. SpaceX is an ambitious venture to create a ...

Get My Altium Designer Free Trial Today.

Get Free Trial