11

Whenever I come across this situation:

unrouted

I feel a strong urge to make a T - joint like this:

routed

However 90 degrees are usually frowned upon. As such what's a better alternative to this T-joint?

If I follow Tyler's suggestion, I'll get this:

acute angle

However this contains an acute angle which is even worse.

bitsmack
  • 16,931
  • 9
  • 54
  • 111
Whiskeyjack
  • 8,286
  • 9
  • 58
  • 99
  • Why not just do like you did with the blue track? have a 45 at the end? – Tyler Jul 29 '16 at 13:44
  • That blue trace is on bottom layer and goes to a through hole pad. However if I do what you are saying, it will form a 135 degree and 45 degree joint. I think acute angle joints are even worse. – Whiskeyjack Jul 29 '16 at 13:47
  • @ whiskeyjack How is it possible to have angle of 135 degree? – Haris778 Jul 29 '16 at 13:49
  • 3
    Possible duplicate of Why is there such a strong preference for 45 degree angles in PCB routing? – Tom Brendlinger Jul 29 '16 at 13:51
  • 2
    In general, 90 degrees connections are not that bad (from a electrical or electromagnetic aspect), neither for manufacturing these days. – Haris778 Jul 29 '16 at 13:51
  • @Haris - I updated the question to show the 135 degree angle. – Whiskeyjack Jul 29 '16 at 13:54
  • is that a resistor + LED? are you asking for this specific case or generally? you could route the trace directly to the pad and then make a derivation from there, so there is no T.. – Wesley Lee Jul 29 '16 at 13:55
  • @Tom - I have seen that answer. However the doubt still remains whether I should go with T joint or whatever Tyler suggested or should I go for another better alternative. I need some expert opinion on this. – Whiskeyjack Jul 29 '16 at 13:56
  • @wesley - I am asking this question in general. – Whiskeyjack Jul 29 '16 at 13:57
  • Yes, make a "T joint". 90 degree angles on PCBs are acceptable in 2016. – Tom Brendlinger Jul 29 '16 at 13:57
  • 2
    Nothing wrong with a T joint. The electrons won't discriminate against them – bitshift Jul 29 '16 at 13:58
  • If you feel uncomfortable then just splay the end a bit to eliminate the inside right angles. – Ignacio Vazquez-Abrams Jul 29 '16 at 14:02
  • @Whiskeyjack If that is 135 degree you meant, than you already have one, and that also is not a problem. Simply make T joint. – Haris778 Jul 29 '16 at 14:04
  • 1
    Thanks guys, for your inputs. I am going ahead with a T Joint. Less headache and looks cleaner as well. – Whiskeyjack Jul 29 '16 at 14:05
  • @bitshift - I was worried what if electrons are not able to figure out which way to go when they reach the junction. :) – Whiskeyjack Jul 29 '16 at 14:08
  • 3
    Everyone is approaching this from a pure electronics standpoint. Allow me to bring in a mechanical engineering consideration into play: If the board will undergo a lot of thermal cycling (or any mechanical cycling if it's a flex circuit), sharp internal corners on the copper traces (like in 90 degree or acute angles) will develop stress concentrations at the interior angle and will be prone to develop fatigue cracking that could eventually sever the trace. For many applications, this is not a concern at all, but if there will be any source of stress cycling, it's an important consideration. – Tristan Jul 29 '16 at 15:08
  • If it isn't high speed 50Mhz+ it doesn't matter, other then a few uOhms from the difference in copper. – Voltage Spike Jul 29 '16 at 17:49
  • I can't agree enough with @Tristan here. If it doesn't hurt, avoid the T joint. The life-span of your PCB will thank you. – Mast Jul 30 '16 at 10:41

6 Answers6

18

There's nothing wrong with a T joint (with two 90° angles).

But if you really want to avoid it, it might be possible to route the entire line through the pad:

route through pad

CL.
  • 19,292
  • 5
  • 42
  • 68
10

Why not take the track point from the resistor pad?

Apologies... my KiCAD is broken (recompiling now)

enter image description here

8

Do not use Tyler's suggestion. You never want to have acute angles, as you seem to know already.

There really isn't anything wrong with T-junctions, especially if you use "teardrops" (or fill in the 90-degree corners):

enter image description here

Personally I just use "Y" junctions, which only have one 90-degree corner:

enter image description here

Take your pick, but don't use Tyler's suggestion. Acute angles can trap etchant which can eat away at the copper over time. This isn't as much of a problem nowadays but it's still best practice to avoid such routing.

DerStrom8
  • 21,314
  • 9
  • 63
  • 97
  • Thanks a lot for posting the answer. Can you please explain which one is trace? blue one between red boundaries or the red ones themselves? – Whiskeyjack Jul 29 '16 at 14:42
  • 1
    Also, red on blue (or vice versa) is harsh to look at. – Dennis Williamson Jul 29 '16 at 17:16
  • It looks like blue is copper and red is bareboard/keepout/lack of copper. – scld Jul 29 '16 at 17:22
  • Sorry guys, these are screenshots of an actual board I'm working on, and those are the default colors. I have a bottom layer pour (the large blue areas) and the thinner blue areas are the bottom layer traces. The red is just you seeing through the clearance between the pour and the traces and seeing the red top layer copper. – DerStrom8 Jul 29 '16 at 18:40
4

Have an acute angle (or 90°) on a PCB is a problem if the junction drive high frequency signal (like communication buss) or a great current amount. This two cases will cause some ECM issue. Otherwise, it's okay to have T junction.

M.Ferru
  • 3,946
  • 3
  • 22
  • 49
3

You can probably get away with 90-degree intersections until you need really thin traces or are routing rf signals. However, this is considered bad practice and I recommend avoiding it.

The other answers are correct; route through pads or add fillers in the inner angles of 90-degree intersections.

Another thing I do is to place an appropriately-sized via at the intersection. Make sure the ring around the via has enough copper to handle the trace's current.

Oh, and don't do this with high-frequency signals :)

bitsmack
  • 16,931
  • 9
  • 54
  • 111
2

Use teardrops to add fillets to such joints. It’s one of the best practices. In Altium, you can apply teardrops to existing traces with Tools » Teardrops » OK.

Altium documentation

Using Teardrops

Teardrops are especially valuable in flex designs to help prevent a crack from forming where the track meets the pad/via or when the drill hole is not in the center of the pad/via. Teardrops are created out of region objects, requiring only one region per teardrop, which can have either straight or curved edges. Teardrops can also be added to the junction of two tracks at both a T-junction and a neck-down junction.

Adding Teardrops to a Design

Teardrops are added (or removed) by selecting Tools » Teardrops from the main menu. When the command is selected the Teardrops dialog will open. Use this dialog to define the mode (adding or removing), and the scope of teardropping as required. Any or all of Vias (and round Thru-Hole Pads), SMD Pads (and non-round Thru-Hole Pads), Tracks, and T-Junctions (and neck-down junctions) can be scoped. Teardropping is created from Region objects instead of Track or Arc objects. This allows each teardrop shape to be created from a single region object, which can have straight or curved edges. If you are working with selected objects only, ensure the Selected only option is enabled.

Altium “Teardrops” configuration

The first protruding line segment (or “line/arc object”) should not be too short to apply teardrops in Altium. With teardrops, it’ll look like this:

PCB traces with teardrops — 2D view PCB traces with teardrops — 3D view PCB traces with teardrops — Actual board

Константин Ван
  • 217
  • 1
  • 7