I heard it is usually better not routing at 90 degree angles. However what about with via, as I've read that it is usually recommended to use one layer for horizontal and another layer for vertical. Can I route safely like the picture below?
\$\begingroup\$
\$\endgroup\$
1
-
4\$\begingroup\$ I asked the same question like 3 years ago. electronics.stackexchange.com/questions/31974/… \$\endgroup\$– efox29Commented Jun 13, 2016 at 21:30
Add a comment
|
3 Answers
\$\begingroup\$
\$\endgroup\$
1
In low frequency designs, the "90 degree" rule is more of a manufacturing issue than an electrical one. Sharp bends can cause acid traps which can cause excessive etching. However in modern PCB manufacturing processes this is not an massive issue.
In high frequency, 90 degree bends cause a noticeable impedance mismatch (in fact 45 degree bends do as well, it's just not as pronounced) because at the corner the trace width changes to be 1.4x wider (think Pythagoras). However this is only really a concern when you start working with signals getting towards and above the GHz range.
From a signal integrity standpoint, whether or not you do the 90 degree bend before a via or do it "through the board" like you show, you will still have at least two 90 degree bends anyway. The trace has to bend 90 degrees into the board, and then bend 90 degree back on the other side. Given it is a cylinder, the 90 degree change in direction on the other side is irrelevant as its effectively a rotation inside the board.
Notice how in cross-section your via is effectively two 90 degree bends. The cross section of it doesn't change regardless of which direction your trace is exiting the via.
This is actually one of the reasons that you have to get very creative and use extreme care when making high frequency vias - and why they are best avoided in HF traces where possible.
You don't say anything about the useful frequency content of the signals on your traces, but given that they are clearly not controlled impedance, it is probably not all that high. In other words, you don't need to worry about what direction you exit the via.
Regardless of the frequency, don't limit yourself to just going horizontal on one layer and vertical on another. Where possible you might as well reduce the number of vias on a trace if for no other reason than vias take up space and make your design larger. For example if you have to go down then across then down again in a trace and there is nothing else in the way, just route the whole trace on the same layer.
answered Jun 13, 2016 at 17:54
-
1\$\begingroup\$ As an example - those four traces exiting the chip on the top? If they can exit the chip in the opposite direction, they don't need vias at all. \$\endgroup\$ Commented Jun 14, 2016 at 7:37
\$\begingroup\$
\$\endgroup\$
4
Personally, I dont see any problem with your layout.
There are some people that suggest that a 90º right angle can generate reflections, but others dont. In both cases, angles will be much less important than the change in impedance with a new via.
In any case, it is something to do with high speed signals. In that case, there are many other issues to take into consideration as well, like the width of the traces, for example.
answered Jun 13, 2016 at 17:35
-
1\$\begingroup\$ It is typically to do with the potential problems during production, such as etchant (acid) traps or under / over etching. For most uses a right angle trace is fine for signal integrity. \$\endgroup\$– DavidCommented Jun 13, 2016 at 17:55
-
\$\begingroup\$ oh, i didnt know it I always use 45 angles because it is cool, and I had no problems with this. But thank you for the info! \$\endgroup\$ Commented Jun 13, 2016 at 18:02
-
1\$\begingroup\$ Just to add (specifically talking about a single trace without a via), although its pretty much covered by the other answer, a 90º right angle definitely can generate reflections. Whether it does or not is entirely dependent on the frequency youre using, and how much that corner changes the impedance. At high frequencies, it will definitely generate reflections (almost all the time). \$\endgroup\$– BeB00Commented Jun 13, 2016 at 21:57
-
\$\begingroup\$ The reason to avoid ANY kind of bend in a high frequency trace is because when you have a 90' bend the copper is wider at the bend which in turn affect impedance. This is why in very high frequency RF circuits it is not uncommon to have no bends at all and instead curve the trace. A curved track has constant width (and impedance). For low frequency (let's say sub 100MHz) it really doesn't matter all that much unless you are designing a precision filter. It is a good idea to practice avoiding right angles and instead "bevel" your corners into 45 degrees angles, just to make a habit of it. \$\endgroup\$ Commented Jun 14, 2016 at 2:52
\$\begingroup\$
\$\endgroup\$
1
Perfectly fine. The right angle rule applies to traces, not vias.
answered Jun 13, 2016 at 17:29
-
2\$\begingroup\$ Incorrect, the via will affect impedance no matter what angle you come out at. If you are designing an impedance matched circuit it's better to avoid vias altogether. \$\endgroup\$ Commented Jun 14, 2016 at 2:56