Manual or Automatic net/wire class net color

Hi Jean-Louis,

You may already know this and it's not automatic but you can do the following to add colors to wires in the schematic:

1. Right click on the wire you would like to edit
2. Select "Properties" at the bottom of the window
3. Select your color/width preferences

It doesn't appear that net classes/or nets in general have an automatic coloring scheme for connected wires.  There may be some funky workaround but I haven't messed with it enough to try and figure one out.  Hopefully someone from the CIrcuitStudio team can comment.

The easyest way to do that is:

Go to Home - Select - Connection than press F11 and modify as you wish. Tip: Save custom colors and add it to selection.

To Altium: You are the the best at navigating designs, please make colors transfer from Schematics to PCB in CircuitStudio and make it pushbutton like F5 in Designer. Please add compiler navigation like in Designer.

You are the best at it and let it shine in CircuitStudio. Do not take that as a negative critic, I love Designer and CircuitStudio.

Hi Jean-Louis,

The Underline Connections command (aka Highlighting Pen) can color the net within one sheet and can be easily navigated to other sheets to color them as well. Please see the screen capture.

Tools > Underline Connections, left-click a wire and the wire highlights or "underlines" with a color.

Press SPACEBAR before clicking and notice the Underline Connections button has changed the color, then click another net to underline it with the next color. There are 7 fixed colors to choose from and these are cycled around each time the space bar is pressed while in the command.

While using the command, hold Ctrl and left-click a Port like INT/CMP shown in the screen capture, then the related schematic sheet opens and that same net is now underlined with the same color.

To clear underlines for the entire project, click the bottom part of the Underline Connections button to Clear Underlines, or press Shift+Ctrl+C.

Best regards,

James Harriman

Altium

Hi Aleksander,

Altium Designer 16 introduced a new feature to take the colors right through the design from Schematic to PCB, using the same colors, with F5 to show Net Color Override. CircuitStudio doesn't have this feature, and has the previous feature called Underline Connections in CircuitStudio, or Highlighting Pen in older Altium Designer versions. The feature isn't currently planned for updating in CircuitStudio.

For others reading this thread: To display colors in PCB in CircuitStudio you need to edit the net of interest and enable the checkbox.

Go to the PCB panel and choose Nets from the drop down. Click <All Nets> and located the net of interest. Double click on the net to change the Connection Color and close the dialog. If the checkbox for the net in the PCB panel is enabled, the PCB will display a checker box pattern of the net color and layer color, that varies visually, depending on the zoom level. When zoomed out it looks like a solid color with the net color. When zoomed in the net color blends with the layer color and zoom in more and both colors are shown with the pattern.

I mention not to forget to uncheck the option, since many people have forgotten that they set the option and then can't get rid of the color for that net.

Best regards,

James Harriman

Altium