# method of locating schematic part on board layout?

In a design with a large number of parts it can be difficult to immediately pin-point a part's location on the board. Is there an easy method of finding a schematic part's location on the board layout?

• Are you talking on a board you're designing, or someone else's design? Jun 23, 2015 at 20:47

It's called 'cross-probing'. In Eagle open the schematic and the corresponding brd, on both interfaces press the eye-shaped icon ("Show Objects"). Now by clicking a specific object in one of the windows it will be highlighted in the second. If you are wondering how to locate a part on the schematic, just type show <part_reference> on the command entry field just above the schematic. The same will work on the PCB view.

• Some vendors charge extra for this feature! It's also worth changing the highlight color (Options->Set->Colors) to make highlighted objects stand out a bit more. Apr 18, 2020 at 11:33

In the SCH, try typing:

sh @ part

which highlights the part with a box, both in SCH and BRD files simultaneously

Use the show tool. This will highlight the corresponding element in both the layout and the schematic.

A good thing to do on dense boards, is renumber the components after the layout is complete. This will make the reference designators read left-right, or top-bottom, as you specify. After this step, you back annotate the renumbering to the schematic. When someone wants to find a part on the board, they can just follow the reference designators until they find it.

It's a little harder if it's not your board because not every designer does this. If there is no rhyme or reason to the reference designators, it's easiest to try to visually break the circuit up into blocks, and go from there.

If Eugene's answer isn't the one you're looking for;

I.e. you mean a finished PCB of which you have only some PDF because you do not have source files, then the answer is nope.

There are many ways to plan components in designs, but there are no guidelines for "you should do X or Y". So some designs will number components from left to right, top to bottom, on the sheet and then they will show up on the board where they make sense, which may seem random to you. Others renumber on final placement. Yet others don't even renumber at all (bad form in my opinion to choose neither).

If you understand the schematic, you can make good educated guesses with some experience: The decoupling cap will be close to the chip, the filtering L will often be at a right angle to a filtering capacitor, which is often across the pins that need the filtered voltage. Etc, etc.