irregular selection on pcb editor (non rectangular)

[SArepairman]

Is it possible to "draw" a selection area on a PCB?

I wanted to move a bunch of parts but they don't fit into a rectangle.

[T3sl4co1l]

S, I
hold shift
draw additive area

Repeat as needed.

Or,
E, E, I
draw subtractive area

Also, O (touching/inside rectangle) and so on.

You may also consider assigning classes for nets or components or whatever, or using rooms.  If nothing else, classes can be selected with a query (on the little query box on the toolbar, or on the PCB Filter panel) such as InComponentClass('classname').

Tim

[dboyer]

S, I
hold shift
draw additive area

Repeat as needed.

Or,
E, E, I
draw subtractive area

Also, O (touching/inside rectangle) and so on.

You may also consider assigning classes for nets or components or whatever, or using rooms.  If nothing else, classes can be selected with a query (on the little query box on the toolbar, or on the PCB Filter panel) such as InComponentClass('classname').

Tim

What is the cleanest way to add a bunch of components to a component class?  I tried using a blanket and a parameter directive but it only seemed to add a net class.  Adding ClassName attributes to each item seems dodgy and gets messed up if I update my parameters from the database. 

[T3sl4co1l]

There's separate directives for net and component classes.  At least, there should be.  (I regularly use net classes, and never use component classes, so..)

You could also push the circuit to a separate sheet, and in Project Options, enable component class generation for sheets.  This is especially handy with hierarchical design and Rooms (all components in the class associated with the Room are dragged with the room).

I normally don't use rooms on a flat design, but if your sheets each have a narrow focus (rather than throwing everything wherever), both the sheet-related component classes and their rooms could be handy for organizing things during early placement.

If nothing else, a dubious method is to assign classes manually on the PCB (Design / Classes), then in Project Options, disable ECO generation for removing component classes, so it remains persistent.  (Note this will screw up the class structure if you later decide to move a component to a different sheet or class.)

Tim

[dboyer]

There's separate directives for net and component classes.  At least, there should be.  (I regularly use net classes, and never use component classes, so..)

This would be perfect but I couldn't find it for the life of me.

You could also push the circuit to a separate sheet, and in Project Options, enable component class generation for sheets.  This is especially handy with hierarchical design and Rooms (all components in the class associated with the Room are dragged with the room).

This would be a solution, I just hate it when tool limitations effect the design in that way.  These are two small related subcircuits that I feel do belong on the same sheet and the software seems so close to making it easy.  I feel like I'm just missing some easy way of doing it.  Thanks for the alternative solutions though!  I'm sure I can make something work acceptably.

[toohec]

As you've already discovered, unfortunately you can't use a blanket directive to assign component classes.  So you are stuck with manually adding the ClassName parameter to each component, or using the automated sheet method mentioned earlier.

Given the potential of losing the ClassName parameter if a symbol is ever updated from the library, I will usually add a note block on my schematic listing the child components under each component class.  Once the schematic is finalized, I can double check the component classes in the parameter manager against the note to make sure no class assignments were lost.  If your notes list reference designators, you'll just have to be careful about annotating.