topic Re: Idea: Automatiacally Arrange Component Names on Board in EAGLE Forum

Idea: Automatiacally Arrange Component Names on Board

Anonymous — Thu, 14 Nov 2019 14:20:09 GMT

Hello, I just finished a pcb layout and really wished that there was a tool/ulp that would automatically arrange the component names on the board. I love to use the hierarchical schematic feature, but it often leads to pretty long component names, thus almost every name reaches into an other component footprint.

I don't know how good this would even work but it'd be a handy feature.

Fabian

Re: Idea: Automatiacally Arrange Component Names on Board

Anonymous — Thu, 14 Nov 2019 16:34:11 GMT

So I suspect that this is a very hard problem, but I am happy to share how I do this quickly.

After you've fully finished laying out your PCB, ignoring the silkscreen, hide all layers except for:

21 (for the top side)

25 (for the top side)

27 (if you include values, for the top side)

29 (shows you where the soldermask is removed so you can avoid placing text there)

46 (mill lines aren't well presented otherwise and you don't want silk over them)

If you so this you get a board where you *cannot* accidentally move a part or trace and can only move the labels (well, and vias, just don't do that, don't know how to avoid it without hiding the vias which are important to know positions of for positioning labels). I do this by hiding "tOrigins" and "bOrigins" because without those there are no handles to click on. I think this gives me a fantastic picture of what the silkscreen will look like.

Switch them to the "b" versions of the layers for the bottom, and flip the board using their tool to see what the bottom will look like. Unfortunately from there I still do it by hand, but this makes it very fast by hiding the extraneous information and making it impossible to accidentally change the board layout.

Re: Idea: Automatiacally Arrange Component Names on Board

rachaelATWH4 — Thu, 14 Nov 2019 16:55:07 GMT

@Anonymous wrote:

If you so this you get a board where you *cannot* accidentally move a part or trace and can only move the labels (well, and vias, just don't do that, don't know how to avoid it without hiding the vias which are important to know positions of for positioning labels).

Your method for silk screen cleanup is similar to mine, but I have a few additional tweaks. To make sure you don't move ANY objects you don't want to move use the selection filter. In this case, when editing the top side silk screen you want to enable just the 'Attribute' selection:

Then issue command :

Display Preset_Top Milling -tKeepout -tRestrict -tDocu

This will give a pretty good view of the top of the board and how the silkscreen will look. You can now move all the reference designators on tNames without any risk of moving anything, components, traces, or vias, they are all safe from being moved.

Now, as per your workflow flip to the bottom view of the board and do the same for that but substituting the bottom equivalents into the above command.

Best Regards,

Rachael

Re: Idea: Automatiacally Arrange Component Names on Board

rachaelATWH4 — Thu, 14 Nov 2019 17:10:09 GMT

@Anonymous wrote:

Hello, I just finished a pcb layout and really wished that there was a tool/ulp that would automatically arrange the component names on the board. I love to use the hierarchical schematic feature, but it often leads to pretty long component names, thus almost every name reaches into an other component footprint.

Hi Fabian,

As @Anonymous says, this would actually be pretty hard to implement something that does an auto cleanup on the reference designators. I like the idea but I don't think we'll see anything soon so I think cleanup is always going to be a bit of a manual task.

There are a few things you can do to reduce the amount of cleanup you need to do in the first place.

1) Have your own clean set of library parts. These should use the vector font consistently for all footprints, and use consistent sizes and positioning so they come in by default as clean as possible.

2) Tidy things up as you go along. Lots of small fixes are easier to stomach than having to spend ages in one hit at the end cleaning things up.

3) Try to avoid using modules. I know the idea sounds good, but the implementation is really lacking and makes a total mess of your reference designators. I just don't use them at all for this very reason. You are better creating groupings of schematic/layout as design blocks and then incorporating them into a master design as many times as needed. This will allow you to reuse layout too and won't mess up your references.

Best Regards,

Rachael