When I first started designing printed circuit boards, it was a very unorganized process. We would create the schematics in our department, and then the system administrators would work their voodoo and transfer all that data from us into the layout department. The layout guys were an even bigger mystery, working all hours of the night and day on these complex Unix machines that supported their CAD layout tools. We would communicate our design intent through documents and spreadsheets followed by meetings and even time spent working with them, and yet somehow it still would get messed up.
The design tools we use now are much better at managing the net connection order between the schematic and the layout. Altium Designer gives us several tools that we can use to verify our schematic and even alter the net rules for layout. This has been very helpful in the communication between engineering and layout and has been a big factor in reducing the errors that used to plague us before. Here are some of the features that we are now using in Altium Designer that have helped us.
Setting up the Error Reporting
Altium Designer gives you a couple of different tools to work with so that you can control the checking of your schematic before you even go into layout with the design. These tools are found in the project options. You can either go to the Project pull-down menu and select “Project Options,” or right-click in a schematic sheet and select it there. As you can see below, the project options menu has many tabs across it. The first tab is the error reporting tab and it allows you to set up how different aspects of your design are going to be reported. Since we are focusing here on managing net connection orders, we’ve scrolled down to the “Violations Associated with Nets” section.
The Project Options menu in Altium Designer
You can set up how Altium Designer will report these different conditions to you by clicking on the colored icons in the “Report Mode” column on the right. The different options available to you are as follows:
- Green: No Report
- Yellow: Warning
- Orange: Error
- Red: Fatal Error
When you click on the colored icon, a drop-down menu will appear where you can select one of four different options as shown below.
Setting the error reporting mode in Altium Designer’s project options
Altium Designer will run all of the checks that you see in the error reporting tab when you compile the schematic. To compile your schematic, go to the “Project” pulldown menu and select “Compile PCB Project.” If your design doesn’t have any errors in it, your schematic design session will not return any messages.
In order to show you what an error looks like, we have removed a portion of the net that connects R1 to Q1 in the picture below and run the compiler. As you can see below, Altium Designer has reported back to us that net “NetC1_1” only has one pin on it. Once I reconnected that net, the compiler ran without any reported errors as it should.
The compiler report showing the missing net error
Working with the Connection Matrix
We’ve got the error reporting set up, and that’s good, but we’re not done with the project options yet so don’t close that menu. The next tab is the “Connection Matrix” which will give you control over how to report your connectivity rules between component pins and net objects such as ports. By clicking on the tab you will see the connection matrix displayed as shown below.
The project options Connection Matrix menu in Altium Designer
As with the error reporting tab the connection matrix tab allows you to set up your reporting for “No Report,” “Warning,” “Error,” and “Fatal Error.” Here though you will repeatedly click on the colored icon to change the reporting. As you can see in the picture below, we’ve clicked on the icon where both the passive pins meet to change it to a red fatal error.
Setting an error level in the Connection Matrix menu
Now when we compile our schematic we can see that the passive pins are now reporting an error. Throughout this schematic where there are passive pins connected to each other, Altium Designer displays an error. Not only does the report window show the errors, but by setting up the Compiler options in the Preferences menu we can also highlight each error with a squiggly line on the schematic sheet.
Passive pins connected together reported as an error
There may be times that you want to allow certain errors to go through, and Altium Designer gives you an option for that as well. By using a command to ignore the electrical rule check (ERC), Altium Designer will not flag that specific object as an error. The feature that you will use for this is in the “Place” pulldown menu, and it is the “Directives > Generic No ERC” command.
To make this work, engage the command and then place the directive symbol that is now on your cursor on the object that you want the compiler to ignore. In this case, we’ve placed the symbol over the lower pin of R1. Now, as you can see below, when we run the compiler the lower pin does not show as an error as it did before.
Passive pins connected together reported as an error with a directive exception
Another portion of the project options menu that will be useful to you is the “Class Generation” tab. Here you can set up Altium Designer to automatically generate net classes for specific parameters as it is being compiled for layout. This is another way that you can help manage the net connections from the schematic.
Using Directives to Help Your Net Connection Order
Another useful use of the directives is to alter the design rules as needed from the schematic. The design rules are usually set up in the PCB document by going to the “Design” pulldown menu in layout and selecting “Rules”. Here you can add new rules and modify existing ones. You also have the option of using the Rules Wizard which is in the same Design pulldown menu. With both the schematic and layout available to you in Altium Designer, jumping into the layout makes working with these rules and easy thing to do. But by using the directives, you can work with the rules from the schematic without ever going into the layout.
As we saw with the “Generic No ERC” directive, go to the “Place” pulldown menu in the schematic and select “Directives > Parameter Set”. With the parameter symbol floating on your cursor, hover over a net and click the mouse button to place it down as shown below. With the goal here of better managing your net connection orders, this will demonstrate to you how to control your PCB layout net rules from the schematic.
Setting a Parameter Directive on a net in Altium Designer
With the parameter set placed on a net, double-click it to bring up its properties. In the property panel you can see different settings for the parameter set including a rules menu which is currently blank. By clicking on the “Add” button you will bring up the “Choose Design Rule Type” menu as shown below.
Choosing a net rule for the parameter directive to use
For our purposes, we will choose the “Routing > Width Constraint” rule by clicking on it and then clicking OK. This will bring up a menu that will allow you to edit the maximum & minimum width rules for the PCB rules from the schematic. Just as you would when working with these rules over on the PCB layout side of Altium Designer, you will make the same changes here. You can alter the minimum, preferred, and maximum widths, and you can set these widths for specific layers in the design.
Setting the width rule for the parameter directive
Looking for software that can manage any layer, produce the PCB design file you need, have easily manipulatable shapes, polygons, and has every step of the design process like a footprint, board design, and schematic view? Altium Designer ensures that all of this is developed thoroughly within an easy-to-learn user interface. No more searching for the right control panel, no more concern over how to connect your design through various PCB footprint edits.
These are just a few of the features that we have found in Altium Designer that have helped us to manage our net connection order. There are plenty of others in this powerful schematic capture tool, and they have all helped us to improve our communication between the schematic and the layout. Altium Designer is a great set of PCB design software, and has made a real difference in our ability to get our designs done faster and with greater accuracy.
Would you like to find out more about how Altium can help you with your schematic creation? Talk to an expert at Altium.
About the AuthorVisit Website More Content by Altium Designer