Cross reference in DesignSpark PCB
How do I have the arrows from and to communicate in two different schemes, to create cross references
CommentsAdd a comment
Here are some more tips on cross references in DesignSpark PCB:
Sheets can't connect if not both part of project. Common error: not checking "Add to open project" when creating a new sheet you intend to be part of project.
The key piece of info is that if a net on one sheet has the same name as the net on another sheet, they are considered part of the same net.
What can confuse people new to DS PCB is that a connection that isn't anchored to something on each end on a sheet will show up in pink as a "dangling connection", even if it is part of a net that has other connections. The To/From components can be used to give these "dangling connections" something to connect their second end to.
(You will find the two TO and FROM components for explicit off-sheet connector symbols in the schema.cml library that DS PCB puts on your pc when it installs.)
Using Add Component, add the TO or FROM component to your sheet. Do not place it right over the end of the dangling line - it won't automatically connect, which can leave you confused. Now select the 'dangling' connection. The use the Add (Schematic) Connection tool to draw from the end of the "dangling" trace to the TO or FROM component. When you make the connection to the TO or FROM component, the 'dangling' connection will no longer be considered dangling, and change from pink to black.
Note one difference between the TO and FROM components is that the TO component displays the name of the other sheet(s) to which the net connects.
For either of the components, you can click on the pad end (single line end) of the arrow, edit the properties (shortcut: Alt-Enter), and toggle the display of the Net name on or off.
If you'd like to build a little catalog of the multi-sheet nets and which sheets they are used on, you can also add a TO component for each net of interest to a sheet without drawing a connection to them. Then right-click on the pad end of each of the TO components you just added, select Add To Net, and select the existing net name. You will then have a TO arrow which lists the other sheets the net appears on, like this:
SCL1 → Sheet5.Sheet3
AC2TX → Sheet5.Sheet3
Note: Any time you add a component to a net which already exists on other sheets, the program will warn you that the net exists already on other sheets. As long as you are intending for it the component to be connected to that global net, go ahead and click Yes. If you instead want it to be on a new, independent net, click No, and you can select a new net name.
You can also right-click on a dangling connection and select Display Net Name. This will attach automatic text with the net name to the dangling connection. You can then position the text to your liking.
One additional note: If I remember correctly, automatically assigned net names are the exception to net names being global accessible. Only user assigned net names are global. If you already have part of a net drawn, using an automatically assigned net name (like N0003), right click on the net, select Change Net (shift - N), and give the net a new name.
User-assigned net names are automatically global across sheets in a project. If you have a net named MyClock on sheet 1, and assign a pin on a component of sheet 2 of the same project to net MyClock, the two will be interconnected.
@BradLevy That is a nice tip, was not aware of that one! "If you'd like to build a little catalog of the multi-sheet nets and which sheets they are used on, you can also add a TO component for each net of interest to a sheet without drawing a connection to them. Then right-click on the pad end of each of the TO components you just added, select Add To Net, and select the existing net name. You will then have a TO arrow which lists the other sheets the net appears on, like this: SCL1 → Sheet5.Sheet3 AC2TX → Sheet5.Sheet3"
The cross referencing or making the net span multiple sheets is done by having the same net name on each sheet. You do not need arrows for this but if you want them for appearance simply creates a schematic only component. Add 'free text' for any source/destination reference if required.