Connect with us


Discussion in 'CAD' started by Antiwin, May 24, 2006.

Scroll to continue with content
  1. Antiwin

    Antiwin Guest

    Does anyone know if exist a library for protel of panasonic electrolytic SMD
    capacitor FC or FK series?
    i mean, they're the typical SMD capacitors but i can't find the footprint
    over all libraries.

  2. you'll have to make the part yourself in pcb library- tools new
  3. Take particular care to note that unless you are using one of the most
    recent versions of Altium Designer (AD 2004 SP4 or AD6), if you use the
    Component Creation Wizard to create a footprint for a surface mount
    capacitor (or a surface mount diode or a surface mount resistor), then the
    pads for that footprint will be incorrectly specified.

    To be more specific, although the appropriate dimensions will be correctly
    specified for each pad's Top layer, that will NOT the case for their Mid and
    Bottom layers as well, which will have ZERO values assigned to them instead.

    Each of those pads will also have a 'Top-Middle-Bottom' value assigned to
    their 'Padstack Mode' property instead of the correct 'Simple' value, and if
    any copy of such a "compromised" component is subsequently flipped to the
    bottom side of a PCB (within a PCB document file), then the properties
    dialog for either of such a component's pads will display ZERO values for
    that pad's X-Size and Y-Size properties. (That is *another* bug; in the case
    of a pad on the Bottom (copper) layer, the values which *should* be
    displayed are those assigned to the pad's Bottom layer - but the values
    which currently *are* being displayed are those assigned to the pad's Top
    layer instead.)

    And yet *another* bug, which "features" in *all* versions of AD 2004 (and
    some or all of the preceding DXP versions as well?), results in the outcome
    that whenever one or more thus "compromised" components are located on the
    bottom side of a PCB, then the Gerber file created from the contents of the
    Bottom Paste Mask layer will be incorrect; images of the "compromised" pads
    will NOT be depicted within that file. Be warned: I have heard of a case
    where a user was bitten by that bug, and who subsequently had to have
    another solder paste stencil manufactured.

    Moral of the story: if you are using a "problematic" version of Altium
    Designer (or earlier major versions), either *don't* use the Component
    Creation Wizard to create footprints for surface mount capacitors, diodes,
    or resistors, or if you do, rectify all of the "rogue" pads before placing
    any instances of any of the footprints concerned into PCB document files.
    (The easiest way would probably be to select both of the pads for each
    footprint concerned, then use the Inspector Panel to change the Layer
    property of those pads from the Top (copper) layer to the MultiLayer layer,
    and then use the Inspector Panel again to change the Layer property of those
    pads from the MultiLayer layer back to the Top (copper) layer again. (Those
    procedures will work because whenever the Layer property of any pad is
    changed from the MultiLayer layer to any other layer, then the pad will
    subsequently ALWAYS acquire a 'Simple' value for its 'Padstack Mode'
    property, which is of course what is desired in these circumstances.))

    Veterans of Altium Designer (and preceding versions, such as DXP, Protel 99
    SE, etc) are of course well aware that there are a number of "gotchas"
    associated with these applications (many of which have still yet to be
    rectified), and as such, subsequently check all Gerber files and NC Drill
    files created from PCB files (prior to sending them to PCB manufacturers)
    very, very, carefully...

    Geoff Harland.

    (Transpose m & s in address
    provided - then also remove
    cuberoot of 10^3 + 9^3 - 1^3.)
  4. Antiwin

    Antiwin Guest

    thanks for your support.
Ask a Question
Want to reply to this thread or ask your own question?
You'll need to choose a username for the site, which only take a couple of moments (here). After that, you can post your question and our members will help you out.
Electronics Point Logo
Continue to site
Quote of the day