メインコンテンツへスキップ

Split scematic over seperate pages

コメント

9件のコメント

  • Steve Stone

    Use the To and From arrow schematic symbols. Help is here:

    https://designspark.zendesk.com/hc/en-us/articles/211424549-How-can-I-add-Net-References- 

     

    The To and From symbols can be on different sheets.

    1
  • Theo Beisch

    Just starting here, coming from EAGLE, still in eval mode if DS or KICAD is the future - and ran across the same topic.

    It generally seems with assigning a net name a net becomes "global" and you can pick it up on another sheet. Show net name (context menu) displays the name. Not sure why that reference component is needed - other than for decoration style.

    A question for the DS experts here: is there a way to annotate these global net labels to identify the sheet pages they are actually referenced to/from - like a cross reference annotation? E.g.: SignalName [1, 2] 

    Thanks ahead!

    PS: Another option I found is the "Closed Bus" feature - adding net labels to a list in a Bus on one page, then Cut and Past the bus over to another sheet and then connect the local parts to the same bus - offers to select the net names and connect to them. Minor hickup: autogenerated net names seem to remain on the schematics page they were generated - so don't use something like "N000x" as it will not connect across (not sur ethat's by intent...).

    So far a plus for DS - KiCAD (5.1 at the time of writing this) to bridge sheets can only either use "global" or what they call "hierarchical" names - these can be exported from a sub sheet to the layer above but that creates quite an ugly number of symbols on e.g. a connector page - though the general idea to keep net names page local seems a good safety feature...

     

    0
  • Oliver King

    Thank you. However, I cannot find the To and From scema in my library for some reason!

    0
  • Steve Stone

    To and From should be in the schema.cml library that comes with DesignSPark PCB. The default location for this in v8.1.1 is C:\Users\Public\Documents\DesignSpark PCB 8.1.1\Library

    If you haven't enabled that path in your library manager or you installed the libraries somewhere else and didn't enable that path you won't be able to find it. If you don't already know how to do this, type CTRL-L (Windows) to bring up the library manager, click the Folders tab and then make sure the folder path is listed and enabled in the top panel, if it isn't there, add it using the Add... button. If it is there but greyed out, select it then click the Folder Enabled checkbox and the schema.cml library should appear in the bottom panel.

    The bottom panel lists all the library files found in all the folder paths.

    0
  • Oliver King

    Hi folks after coming back to this project I am still struggling! I have two schematics spanned over two pages, and I cannot get the net's to behave globally. Not sure what I am doing wrong but they are part of the same project. Reading Theo's response above is this something to do with auto-generated net names?

    What can I actively do to correct this?

    0
  • Boss .

    I don't use "To" or "From".

    Simply name the net on sheet 1 and then on sheet 2 select the required "same net" to highlight, right click and select "Change net" and select the named net (from sheet 1) from the list of all the nets in the project.

    There may be different behaviour with the auto generated names, but I name each net for clarity and have no issues.

    The ChipKits exmple project does it this way without "to" and "from".

    0
  • Brad Levy

    Oliver, auto-generated net names are local to the sheet. Only user-entered net names are global.

    You can rename the auto-named net on each sheet it appears on to make it global.

     

    1
  • Brad Levy

    Theo and Oliver, here are some of my notes regarding global nets, including some tips about building are cross-reference list:

    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
  • Oliver King

    Thanks, folks all sorted now. It's a pain that you have to assign your own names but there you go!

    0

サインインしてコメントを残してください。