irregular selection on pcb editor (non rectangular) - Page 1
Forum section: electronics / general

author: SArepairman
author_rank: Frequent Contributor
timestamp: June 29, 2014, 06:42:09 am
content: 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.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: June 29, 2014, 06:52:55 am
content: S, Ihold shiftdraw additive areaRepeat as needed.Or,E, E, Idraw subtractive areaAlso, 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

author: dboyer
author_rank: Contributor
timestamp: July 01, 2014, 03:06:23 pm
content: Quote from: T3sl4co1l on June 29, 2014, 06:52:55 amWhat 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.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: July 02, 2014, 04:41:43 am
content: 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

author: dboyer
author_rank: Contributor
timestamp: July 02, 2014, 04:06:48 pm
content: Quote from: T3sl4co1l on July 02, 2014, 04:41:43 amThis would be perfect but I couldn't find it for the life of me.Quote from: T3sl4co1l on July 02, 2014, 04:41:43 amThis 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 seemssoclose 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.

author: toohec
author_rank: Contributor
timestamp: July 03, 2014, 01:34:13 am
content: 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.