Skip to main content

TO symbol in schema.cml

Comments

6 comments

  • Official comment
    DesignSpark PCB

    Christophe's issue was identified as a corruption within the library which has now been restored and working.

    Brads issue will be tested to try to replicate.

    The "TO" component has not been changed and is part of DesignSpark PCB v9, if anyone has any issues we would like to investigate and resolve so please contact our support team using https://designspark.zendesk.com/hc/en-us/requests/new

  • Boss .

    As this is a user-supported forum you would be better off raising a support ticket.

    https://designspark.zendesk.com/hc/en-us/requests/new

    Did you accidentally delete the symbol? It's unusual for any to be missing if the library is enabled.
    As a faster fix, if you had an earlier version installed previously you could map the library (in Public documents).

    Or if you use Windows Add/Remove programs I think you can do a repair.

    0
  • Michael Harvey

    I assume "TO" means a connection in the schematic to some other point in the same schematic page or other page without having a line (wire) to connect the points visually displayed on the schematic..

    I often use more than one schematic page and connections between the pages can be done by 

    (1) naming the net the same between the pages and use text to indicate the connection

    (2) use bus bar. Add Bus <Ctrl B> (this makes it a lot more tidy and is the easier and best option)

    The example attached means I can <Copy><Paste> the SD Card to a new project.

    Another tidy habit is to always name your nets. (simple connections between two components can keep the default system generated net name. Example attached. I hope I have not misunderstood the meaning of your "TO".

     

    1
  • Brad Levy

    I haven't checked V9.0, but I did double-check the libraries of DS PCB 8.1.3 and the trial version of DS PCB PRO and it was there in both.

    Note that the TO component is in schema.cml, but the schematic symbol is in discrete.ssl. 

    If you don't have the discrete.ssl library enabled, it won't be able to find the schematic symbol when you go to use the TO component (which references the TO symbol).

    (Both of those libraries are in the Library (not Library/User) folder of the DS PCB version.)


    As to Michael's comment, yes, explicitly naming your nets is always a good idea, and required if you want the net to connect across multiple sheets. Default (auto-generated) net names are local to a sheet. But you do not have to use a bus for global nets.  And there are some useful tricks using the TO symbol. Here are some of my notes from way back:

    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.
    Here is a technique which I just tested using the chipKIT Max32 example project as a testbed:

    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:

    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. If you want explicit off-sheet connector symbols, you'll find two components, named FROM and TO, in the schema.cml library, that can be used for those.

     



    0
  • Christophe

    Thank you Brad for your comment, I verified that discrete library is enable and it is. In the "Add component" windows, the schema library has no component and in the discrete library, there is no TO or FROM component. Do you know how can I get this symbol in the add component windows ?

    Thank you

    Christophe

    0
  • Brad Levy

    Which version of DS PCB are you using?

    I did some exploring last night, and found issues when trying to use the TO component with DS PCB 8.1.3.

    The component itself is quite simple, an arrow with a pad at one end, and Netsheets attribute of the pad being clicked as visible in the schematic symbol editor. I created my own similar one with a slightly different appearance. But when I tried to use either in the ChipKitMax32 sample project, it crashed. Then I tried it in the free trial version of DS PCB PRO, and it didn't crash, but had an anomaly not displaying the sheet references initially until I made another change in the schematic.

    So maybe it was removed at some point for being problematic?   Hmm...

    Most of my designs are small enough that I don't use multi-sheet schematics much. But if I did, the sheet cross-referencing ability of the TO component would be nice to have.

    -Brad  (just another user)

     

    0

Please sign in to leave a comment.