Schematic Library components pin designator sorting

[vincei]

How do you stop Altium designer sorting component library pins by designator? I have a PGA part (retro) that has 175 pins, labeled A01 thru S16. I use these designators so that I match my schematic to the datasheet to the device PCB footprint to make sure everything is right. I have entered all the display names per the data sheet, however, no matter what I do Altium sorts the pins by designator. I want them sorted by Display name so that things like address, databus and other control signals are grouped together regardless of their designator. Even using the group function of Altium the pins are still subsorted by designator which is, well, why?!?

How do I make it show A01  thru A31 sorted in the order that makes life drawing the Scematic easier? See the second image.

I'm new to Altium so that and maybe me just being thick 

-Vince

Altium 19.1.8, Don't want to upgrade to 20 yet unless it makes this easier :-)

[T3sl4co1l]

This can be done with selections/queries and List or Inspector (Property) assignment.

List:
Select the pins.
Open List panel/dialog.  Set: "Edit", "selected objects", from "current component".  Include "all types".
Sort by Y1. Select and CTRL+C (copy) the coordinates.
Sort by Name. Paste Y1 coordinates.

Inspector:
Select the pins.
Open Inspector/Properties.
In Y1, enter: Copy(Name, 2, 99)*10
Move pins into desired location(s).

The list method is pretty obvious, just swapping around tables.  Synergize with Excel if you need more power (or learn scripting).

The latter expression is the tricky stuff you might not be expecting -- or know very well how to use.  Sadly, objects have three different names in Altium, and they don't always make sense.  I haven't seen anywhere these are tallied.   You read one description in the object dialog or Inspector panel / Property dialog, but that's different from the reference used in an expression.  For example, here you can reference an object's name field by "Name", but its designator is "Pin_Designator".  But on the Query panel, it's "Name" or "PinDesignator".

Also, note that, to use an expression on a text field, you need to click the "..." and enter it on the Formula tab.  Substitution expressions ("{xxx=yyy}") can be entered directly or created in the "..." Batch Replace tab.

Tim

[vincei]

Thanks, Tim. I'll give this a try. Here I was thinking it would be something simple and obvious  Used excel and some bash shell one liners to generate the CSV for pasting the pin definitions from the datasheet into the symbol wizard so scripting shouldn't be too much of a pain :-)

Cheers,
Vince

[vincei]

Thanks, that worked. As a newbie it took me a little time to figure out exactly  what you were saying and implement it.

Cheers!
Vince