メインコンテンツへスキップ

Symbol I created not seen by Add Component

コメント

6件のコメント

  • Brad Levy

    You have to create a component (on the Components tab of the library manager) before you can see/use a part in the schematic editor or PCB editor. A Component can be Schematic-only (if it has a schematic symbol associated with it, but not a PCB footprint), PCB-only (if it has a PCB footprint associated with it, but not a schematic symbol), or normal (both a schematic symbol and a PCB footprint associated with it).

    Schematic-only components can only be used on schematics. PCB-only components can only be used on PCBs. Normal components can be used on schematics and PCBs, and will automatically be found when you convert a schematic to a PCB. An example of a schematic-only symbol is a voltage or ground network reference. These refer to networks on the schematic (that will be carried over to the PCB design), but they don't represent a physical component that has to be installed. Another example would be a line graphic (like a design sign-off record box) that should appear on the schematic, but has no counterpart on the PCB.

    Examples of PCB-only components would be mounting holes or fiducial marks. These can be important as part of manufacturing and mounting the PCB, but wouldn't be used on the schematic.

    This chart may help you understand the relationships between the different libraries and components:

    0
  • Garry Collins

    Hi Brad.

    Much appreciated, I now understand. I am used to symbols essentially being standalone entities containing all the information necessary to call the relevant footprint during the packaging process when creating the PCB from the schematic.

    Is this sort of information available somewhere, video tutorials are all well and good, but it can be much quicker to access this information in an indexed repository such as an old fashioned manual.

    Again, many thanks.

    Garry

    0
  • Garry Collins

    Hi Brad.

    Thanks, that worked perfectly.

    As this is an RS part without a component in the DesignSpark library, is there any process for submitting a component for inclusion in the public libraries?

    Thanks,

    Garry.

    0
  • DesignSpark PCB

    Hi Garry, we have videos and FAQ's here

    https://designspark.zendesk.com/hc/en-us/categories/201145765-DesignSpark-PCB 

    PCB Part Library used with Library Loader and a component search engine provides our online component resource. Any parts not found can be requested.

    Simple components are also easily and quickly created with the Wizards as detailed in the FAQ's in the above URL.

    0
  • Brad Levy

    Hi Garry,

    The built-in help, available via the F1 key or from the Help submenu of the main menu, is the manual. It is fairly complete, but not always organized in the order you'd want to read the material. Fortunately the Help lets you search for keywords or topics, in addition to the already indexed terms. In this case, the relationship between components, schematic symbols, and PCB symbols is under the Library Structure topic. This forum is a good source for information about why some things are the way they are in DS PCB, and how to best utilize them.

    The reason for having the schematic symbol and PCB footprint libraries (instead of just the component libraries) is to allow re-use of the symbols and footprints.

    If you go to a order parts, there are thousands of different resistors (components) that all use the same schematic symbol. The same is true for other components like capacitors, transistors, logic gates, op amps, etc. By sharing a symbol from the schematic symbol library between many Components, the symbol only has to be drawn once, and thousands of copies of it don't have to be stored in the libraries. You can also have more than one schematic symbol per Component. A dual op amp or an eight-resistor array can be considered single components made up of (in this case) two or eight functional elements, which DS PCB refers to as gates (even if they are analog and not logic). The multiple gates of a component need not be immediately adjacent or even on the same sheet of the schematic.

    Likewise, there are many components that share the same PCB footprint. The footprint only needs to be stored in the PCB symbol library once, and can be used by each of those components. (It is also possible to have multiple PCB footprints associated with the same component, for parts that are available in more than one package style. In this case, there will be a separate pin mapping table for each package style used.)

    Another point - when you add a Component from the library to a schematic or PCB, a copy of the component plus the corresponding symbol is stored in the schematic or PCB file, so the schematic and PCB files are self-contained. If you take the schematic and PCB file to another computer that doesn't have the libraries those Components came from, the files are still editable.

    0
  • Brad Levy

    As far as a public library of user-contributed components, there isn't currently an officially maintained one.  There are legacy ones installed with but DS PCB, but not automatically enabled. One issue with any library is quality control. I highly recommend users of any PCB program (not just DS PCB) do some verification of components against the data sheet.

    You could make it available to other searching here by uploading it as a zip file here. Use a subject line something like  User Contribution: Part name.
    Include in the post any special tips on usage, and (if it includes a PCB symbol) whether boards have been made with it and checked with an actual part.

    0

ログインしてコメントを残してください。