edit the decal in a text editor, you can delete the outline in question in a text editor
use the asscii file you have zipped
I use 2007, so I am not sure if the format is the same but what I see is an open(as opposed to a closed shape, a square for example) line on layer -2 (!!!)
at least that is what it is according to the 2007 format
closed 5 0.25 -2 -1
the -2 is the layer (at least in 2007 it would be)
see plib_ascii.pdf (could be a different name in V9) for the library ascii specification
When I remove the section:
CLOSED 5 0.25 -2 -1
From the file I get the following error when importing the modified file:
Bad drawing piece type T0 <EDSTLZ1555/2>
T0 0 0 0 1
I exported this using 9.3.1. According to the Parts Library ASCII format spec
Each piece entry consists of a header line followed by a list of line segment or arc segment
type numcoord width layer linestyle
x y (format for line segment)
x y ab aa ax1 ay1 ax2 ay2 (format for arcs)
type Type of piece Valid values are OPEN, CLOSED, CIRCLE, COPOPN, COPCLS, COPCIR, BRDCUT, BRDCCO, KPTCLS, KPTCIR, or TAG. (The TAG piece is used to combine coppers and copper cutouts inside the part decal into one item. It does not contain any coordinates and is used as either opening or close bracket. TAGs are also used to combine dimension pieces into a dimension drawing.)
numcoord Number of coordinates defining the item For open items, this is the number of corners. For closed line items, it is the number of corners plus one (to return to the starting corner). Circles have two corners that define opposite ends of any diameter. For TAGs,
width Line width of all segments in the piece Values range from 0 to 0.25 inches, expressed in the selected units of the item.
For TAGs, 0 (zero).
layer Numeric layer number for use in PADS Layout. Values range from 0 to 250. A layer value of zero means all layers. The layer number is ignored in PADS Logic.
For TAGs, the layer value specifies the TAG “type”:
• 1 means an “opening bracket”, that is, start of the group.
• 0 means a “closing bracket,”, that is, end of the group.
From this I take it the piece I am trying to remove is on layer "-2". How can you have a -2 layer
As a follow-up to this.
If I select the component in the PCB design. I then RMB and select edit decal to try and remove this. I cannot select this mystery shape, no matter what my selection filter is set to.
Did you check your layer color setup in the Decal Editor? This mystery shape may be on a layer that isn't displaying. I've had some odd color definitions coming up lately. My default colors don't seem to apply anymore. That 'layer -2' is pretty mysterious.
in addition to removing the offending line piece like you have done, you also need to edit the line:
EDSTLZ1555/2 M 0 0 0 3 10
change the 10 to a 9
it is the number of pieces
so if you delete one piece, lower the count by one
That was it (changing the piece count 10 to 9). I knew I was missing something as the file structure is pretty simple if you don't mess it up.