Library

you'll have to make the part yourself in pcb library- tools new component....

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...

Regards, Geoff Harland. g snipped-for-privacy@optum12net.cos.au (Transpose m & s in address provided - then also remove cuberoot of 10^3 + 9^3 - 1^3.)

"martin.shoebridge" wrote

footprint

thanks for your support.