Alternate method for finding PCB components among the "pile" - Page 1
Forum section: electronics / general

author: jmarkwolf
author_rank: Regular Contributor
timestamp: October 19, 2017, 12:22:05 pm
content: As I progress through my first end-to-end Circuit Studio design, I'm finding more dubious "features".Finding schematic parts works fine, but I haven't found a way to find individual PCB components in a pile of parts such as after doing a "update PCB document". The cross probe feature doesn't work well if the part of interest is small and the pile is large (can't see the highlighted part).Altium Designer has a short cut which is to move the cursor where you want the part, then hit 'M' & 'C' (short for Move Components) then type the reference designator, and the part will snap, from wherever it is, to the current location of the cursor. It's much easier for digging parts out of the pile of parts.Is anyone aware of an easier way to find specific PCB parts in the pile of parts?

author: voltsandjolts
author_rank: Unknown
timestamp: October 19, 2017, 01:58:29 pm
content: Type the designator into the search box at the top right of the CS window.

author: jmarkwolf
author_rank: Regular Contributor
timestamp: October 19, 2017, 03:12:27 pm
content: Quote from: voltsandjolts on October 19, 2017, 01:58:29 pmI tried that when looking for "C18" and, if I remember correctly, as soon as I typed the "C" it tried launching me into some help docs or something. I'll try again more carefully.

author: slowertech
author_rank: Contributor
timestamp: October 19, 2017, 06:38:09 pm
content: I usually type in and select "Cross Select Mode" within the search box, select the part or parts in order that I want to move in the layout. In the layout tab I will type out "Reposition Selected Components" and it will move the part to your mouse cursor within the layout and if you have selected multiple parts within the schematic then after placing a part in the layout it will move on to the next part in the order you had selected them.Hope this helps!

author: jmarkwolf
author_rank: Regular Contributor
timestamp: October 19, 2017, 10:22:56 pm
content: Thanks VoltsandJoltsIt does indeed work. Odd that it lists all parts of the same designator for all open projects, though.When I first tried it, upon typing the first character it dropped a long list of items and docs that had nothing to do with what I was trying to accomplish, so I moved along thinking it wasn't working.Also odd that the search window on the SchDoc side only directs you back to results on the PcbDoc side.But at least the SchDoc side has a "real" menu item for finding parts (Tools/Find/JumpToComponent). Makes you wonder if the Schematic capture team talks to the PCB Layout team! Wish they had left the Altium menu's intact and just grayed out features they didn't want Circuit Studio to have.Hopefully they'll sort it out for a subsequent release.

author: jmarkwolf
author_rank: Regular Contributor
timestamp: October 19, 2017, 11:51:41 pm
content: Quote from: slowertech on October 19, 2017, 06:38:09 pmHi SlowerTechHow on earth did you figure that out? It's not working for me, maybe I'm phat fingering something.

author: slowertech
author_rank: Contributor
timestamp: October 20, 2017, 12:42:17 am
content: Quote from: jmarkwolf on October 19, 2017, 11:51:41 pmHaha, got irritated and just started trying to type things out.Have not tried to make sure that this part is not important with Circuit Studio but I keep the schematics in one window and the layout in a separate window so I can see both at the same time.Also I forgot to mention that I need to type in and select "Cross Select Mode" 2 times before it functions.Let me know if that works for you.

author: songshome
author_rank: Newbie
timestamp: October 20, 2017, 03:41:22 pm
content: You must have cross select mode enabled both in sch and pcb. Cross select is under Home tab - Select - cross select. Shortcut alt, h, s cursor down and enter. Or you can type in search box.If you have pcb in 3D mode, it works too. That is the beauty. Just enable PCB panel with components view active. After selecting schematic parts, footprints will become selected too. Now you can just rightclick on one off selected parts in panel and - Reposition components. I love this software.And another beauty: Repositon components will work in order of selecting the components in schematics. For example: opamp, bypass caps, feedback resitor.... It can't be better.

author: slowertech
author_rank: Contributor
timestamp: October 21, 2017, 01:34:09 am
content: Quote from: songshome on October 20, 2017, 03:41:22 pmHaha wow. This entire time I never knew it was under the home tab. Thanks!