Indicating Plugged Vias

Making PCB Layouts, Manual routing, Auto-routing, Copper pouring, Updating from Schematic, Manufacturing Output
Post Reply
Message
Author
donwynne
Posts: 1
Joined: 09 Mar 2022, 19:16

Indicating Plugged Vias

#1 Post by donwynne » 09 Mar 2022, 19:23

Is there a good way to indicate on a separate layer all vias on a PCB that will need to be filled/plugged with non-conductive epoxy? I haven't found any direct options for this for individual vias or for via styles.

Historically I've handled this creating a new non-signal layer and adding circles on the precise location of each via that needs to be filled. This lets me create a gerber layer that specifically calls out only the plugged vias. However, my PCB in question has several hundred vias placed on it, so anything I can do to avoid manually placing an indicator on each individual via would be helpful.
Last edited by donwynne on 11 Sep 2022, 18:53, edited 1 time in total.

Tomg
Expert
Posts: 2028
Joined: 20 Jun 2015, 07:39

Re: Indicating Plugged Vias

#2 Post by Tomg » 10 Mar 2022, 06:03

EDIT: Here's a shortened version of the original procedure that will produce a new layer of circles surrounding the vias that need to be plugged...

1) Create a new, Non-Signal layer named "Plugged Via Locator" and give it a unique color.
2) Set the Top layer as the working layer and unpour its copper pours.
3) In the main menu click on File > Export > Gerber... to bring up the "Export Gerber" dialog window. If another window appears with a warning about unpoured copper pours, ignore it by clicking on its [OK] button.
4) In the "Export Gerber" dialog window select/highlight the Top layer and take note of the default settings before continuing (e.g. take a screen shot and print it out if necessary) as you will need to restore these settings in step 5 below. Now, deselect (uncheck) all Objects except for [x]Vias, click on the [Export Layer] button to bring up the "Save As" dialog window, enter a unique file name (e.g. "Plugged Via Locator") and save it to a convenient folder such as the desktop.
5) Returning to the "Export Gerber" dialog window, restore the original settings and then click on its [Close] button.

6) In the main menu click on File > Import > Gerber... to bring up the "Open" dialog window, locate and select/highlight the newly-created Gerber file and click on the [Open] button to bring up the "Source Gerber File" dialog window.
7) In the "Source Gerber File" dialog window set Import Mode: "Add", Convert to: "Plugged Via Locator", click on the [Import] button and turn off the Top, Bottom and any other copper layers (inner layers) if they exist.
8) In the main menu click on Edit > Edit Selection... to bring up the "Edit Selection" dialog window, enable only [x]Shapes/Pictures, choose "Plugged Via Locator" in its drop-list and click on the [OK] button.
9) Right-click on one of the selected/highlighted objects, choose Properties..." in the context menu to bring up the "Shape Properties" dialog window, set the Type: drop-list to "Board Cutout", set both "Width:" and "Height:" to one identical value slightly larger than the via pad size and click on the [OK] button.
10) With all modified objects still selected/highlighted, right-click on one of them, choose "Properties..." in the context menu to bring up the "Shape Properties" dialog window once more, set the Type: drop-list back to "Plugged Via Locator" and click on the [OK] button.

11) Deselect everything by returning to the Default Mode (click in an empty area), delete any Plugged Via Indicator circle that doesn't apply, add instructional text you think should be included in the Plugged Via Locator layer, turn on the Top, Bottom and any other copper layers (inner layers) if they exist and repour all copper pours.
12) Resave the PCB file.

Here's an example...
pvl.png
pvl.png (46.7 KiB) Viewed 126 times
Tom

Post Reply