Can I denote a track as 'sacrificial' on the circuit?

Drawing Schematics, Hierarchical Design, BOM, Exporting net-lists, etc.
Post Reply
Message
Author
greiginsydney
Posts: 8
Joined: 03 Sep 2020, 03:30

Can I denote a track as 'sacrificial' on the circuit?

#1 Post by greiginsydney » 09 Jan 2021, 18:23

Hi All,

The circuit and board I'm working on has provision for an optional changeover relay.

It won't be used in a lot of builds, so I am proposing adding what I'm calling a 'sacrifical' track between the Common and NC pins so the board functions by default, without needing links to stand in for the NC connection. The constructor will cut this track when they add the relay.

Is there a way I can capture this on the schematic? I don't want it to have pads, just perhaps something that looks like this on the schematic:

"-----X-----"

... and I can add a piece of text next to it that says "cut this track if using the relay".

Thanks,



Greig.

Alex
Technical Support
Posts: 3501
Joined: 14 Jun 2010, 06:43

Re: Can I denote a track as 'sacrificial' on the circuit?

#2 Post by Alex » 11 Jan 2021, 10:27

You can create PCB jumper. It can be a component with two pins and attached pattern with two pads that are normally connected by copper shape.

SoundMod
Posts: 72
Joined: 15 Feb 2016, 12:47

Re: Can I denote a track as 'sacrificial' on the circuit?

#3 Post by SoundMod » 11 Jan 2021, 10:48

Here is the workaround;

1. In component editor, Create a custom 2 pin symbol (in your case something like -----X------ ) in the component editor
2. Name that symbol whatever you want but also think to append something to denote the width of the trace. For example, "SACRIFICIAL_W12" for a trace of 12MIL or "SACRIFICIAL_W18" for a trace of 18MIL.
3. Create a custom 2 pad footprint, match the width of your pad to the width of the desire "SACRIFICIAL" trace.
4. Select one of the pad > Right Click > Mask/Paste Settings...
5. In state section;
A) Change the state of Top Solder Mask from "Common State" to "Tented".
B) At the bottom of the Mask/Paste settings popup window, change the drop down menu "Apply to" to "Similar Pads"
C) Hit the OK Button

Now, if done correctly both pads should be covered by soldermask.

6. Now you can draw a line on the copper layer between both pads to link them together.

Basically, you can create many type of PCB jumper with that method.
However be aware that the DRC will throw you error because both pad will be connected on 2 different net in the schematic and that Diptrace will see the line linking both pad as a short-circuit.

I hope that Diptrace Team will add a "Net Tie" feature to avoid that problem.

greiginsydney
Posts: 8
Joined: 03 Sep 2020, 03:30

Re: Can I denote a track as 'sacrificial' on the circuit?

#4 Post by greiginsydney » 11 Jan 2021, 20:23

Thanks, that worked well! Very sneaky.

And interestingly, no DRC errors.

DipTrace-LK-cct.jpg
DipTrace-Rly-CUT.jpg

- Greig.
You do not have the required permissions to view the files attached to this post.

Post Reply