Will I have any trouble routing the traces in this way? (VCC and GND)
Is it OK considering that the entire circuit current is under 50mA?
Asked
Active
Viewed 5,717 times
26
-
34By the naming convention those look like connectors of some sort. If so, and if the pin order is not pre-determined, I would recommend putting Vcc in the middle and ground and data on either side so incorrect insertion does not reverse the power to whatever it connects to. – Trevor_G Mar 28 '18 at 16:23
-
Thanks for the tip, I never thought about it. Those are connectors for sensors like dht21 and such that dont come with a proper connector, only bare wires – Lucas Alexandre Mar 28 '18 at 18:19
-
3For sheer function, it should be no problem. If you struggle with passing EMC, this may or may not turn out to be a problem for high speed signals. Never encountered it myself, just been told about the phenomenon in an EMC class. – winny Mar 28 '18 at 19:14
-
Saw this on the hot network question list and misread it as "traceroute through a pad" and was wondering how that would work... – Michael Mar 28 '18 at 21:09
-
2I would only warn about mechanical stress, connectors are among the first things to be torn out by mistake. Should it happen then it could brake the trace and make the hole circuit fail. So if you have the oportunity i would not make it go through the pad if you have free space. – ndelucca Mar 29 '18 at 12:29
-
This is perfectly normal. On some CAD systems, you have to click on each pad as you place the track to ensure that the DRC function will see a connection between track and pad. – Peter Bennett Mar 30 '18 at 18:58
6 Answers
55
There is no problem routing traces through pads (like you have done). Be aware when routing power/GND of the current that will be travelling through these traces. This will dictate trace thickness. In addition, search for "power planes", "ground pours" for more information.
I can see where your confusion may come from. I'm not a fan of how Eagle renders traces connecting or passing through vias/pads.
When you do this:
The thickness of the annular ring needs to be considered to ensure that it can carry the required current.
-
11Good point about the current capacity. If something is soldered into the hole then there will be a lot more cross section available. But then what if it doesn't get populated ? – Criggie Mar 29 '18 at 01:01
-
16
-
-
1
14
No, it is not a problem routing through a pad. You might wish to consider adding ground and power planes to the design.
Lior Bilia
- 7,282
- 1
- 20
- 30
9
This should not be a problem if the pad is used, i.e. soldered before use. That will increase the current carrying capacity many times. Additionally, each side of the ring looks about as thick as the trace, so even without soldering, current capacity has been doubled.
But what does current carrying capacity really mean anyway? The pad is tiny, there will hardly be any voltage drop across it. And because it has greater surface area compared to volume, it will heat up less than the track. So unless there are a bunch of pads on the track, there is no cause to worry.
The real problem of course is if the pad is small, drilled and not soldered. In this case a track might be broken due to a bad drill bit. And, may not be noticed in a complex layout.
Much more importantly, an undersized pad may not be mechanically strong, especially when connectors are involved. I would widen the tracks on both sides of the pad just for the mechanical strength alone. Has saved me many times. The epoxy that holds the copper to the board can only take so much. Also make sure the drill holes fit tight.
Indraneel
- 2,117
- 1
- 17
- 24
-
the trace width is 24mils. Do you think i should thicken it even further? if yes, only in the area near the pad? – Lucas Alexandre Mar 28 '18 at 19:12
-
1Trace thickness is determined by the current and heat dissipation the trace needs to handle, and indirectly by whether the traces are on the top or bottom, or buried. 24 mils is gigantic for typical digital signals, but you'll need to figure your Vcc/GND current to determine adequate trace width. – Bort Mar 28 '18 at 20:15
-
2If the connector will be subjected to repeated stress (frequent insertions, bent wires in enclosure etc.) I would thicken the track only near the connector pad, maybe about 5mm either side. It's fine as long as it does not violate clearance. Less of an issue in plated holes with pads on both sides, but why risk it? I'd think 0.8mm as safe (~32mil). Of course, even 0.1mm trace would be overkill for humidity sensor current, but that's not the issue here. – Indraneel Mar 28 '18 at 20:38
5
If the connections to those pins are the same VCC and same ground you will have no issues.
Physically the copper track will only go as far as the pad it wont actually be left hanging over the hole upon manufacture.
Pop24
- 680
- 1
- 5
- 17
3
In relation to current, your trace is not 24mils (0.61mm) passing across the hole. This is a custom PCB, not one of those cheapo Veroboards. It's actually about 3.81mm (150mils). You need to consider that if your PCB is the standard 1.6mm thickness, and the hole is through plated, the hole has tinning on it's cylindrical perimeter. Like so:-
The implication is that whatever your actual trace width is approaching the hole, even if it was a micron and the annular width was a micron, you'd still have 3.2mm of copper along /across the depth of the hole. So it doesn't really matter if the hole is filled or not. It's actually one of the highest current capacity parts of your copper layer unless you have something > 126mils wide.
Paul Uszak
- 7,327
- 5
- 37
- 69
1
As mentioned earlier, use Ground planes. In Eagle, draw a polygon around the entire board and Name it Gnd. Do that for both the Top and Bottom layers. Rip up any Gnd traces you have. Add Vias in spots around the board and Name them Gnd as well to connect the top & bottom Ground layers.
On a 2 layer board, creating a Vcc (5V, or 3.3V)) is harder, those are usually routed as traces.
CrossRoads
- 3,453
- 1
- 6
- 14