EMRFD Message Archive 8730

Message Date From Subject
8730 2013-06-13 21:28:13 Dave Miller Microstrip to board edge desgin rule
I am having a discussion with an associate on running a impedance controlled RF trace on a board. I cannot seem to locate a definitive reference to how close you can run the trace to the edge of the board.
I am concerned about both impedance matching and radiation.
References are appreciated. ;-)

The only thing I have found seems to say that the ground plane (lower layer 2 layer board) should extend 1 x ( where x is height) closer to the board than the trace.

So if the board thickness was 0.062" and the Signal trace was .100" from edge of board,the ground plane should be extend within 0.038" of the edge of PCB. ?


The board has ground infill on the inner side.

I am not expert but seems to me looking at all microstrip references they seem to assume that the trace has a ground plane that extends beyond the trace edges.

Thanks
Dave
VE7PKE
8731 2013-06-13 22:22:38 ka7exm Re: Microstrip to board edge desgin rule
Dave:

I wonder what operating frequency you are operating at. In addition, the dielectric constant of the material would be helpful to note.

In general, I've used 3x the width of the trace (or the thickness of the dielectric on either side of the trace as a very quick spacing to any other trace. The bigger thing to watch out for is the shape of the nearby structures. For example if you have a trace nearby of some particular length, you will get absorpti
8732 2013-06-14 03:05:31 ha5rxz Re: Microstrip to board edge desgin rule
Agreed, three times the width of the trace as a minimum spacing requirement.

Peter HA5RXZ

8734 2013-06-14 17:52:51 Dave Miller Re: Microstrip to board edge desgin rule
Thanks for this information.
I guess I am not explaining my question. or understanding the responses.

My question is. if you have a single trace over a groundplane how much must the ground plane extend on either side of the trace for it to be the calculated impedance and minimize radiation.

I will post a picture in the photos section.
Blue is ground plane on bottom of board.
Red it Top Trace.
What is he dimension shown as 100 mil
8735 2013-06-14 23:09:40 Kerry Re: Microstrip to board edge desgin rule
Good question; there is not much on this aspect of microstrip that I can find.

The width of the ground plane is, in theory, infinite but the effect drops-off with distance from the centreline of the microstrip and, at some point, becomes negligible (a word that means different things to different people :) ).

This "tapering" effect is analogous to skin-depth where one skin-depth is defined as the depth at which the current has fallen to about 0.37 times the current at the surface but current still flows at greater depths.

I did find this;

http://www.google.com.au/url?sa=t&rct=j&q=&esrc=s&source=web&cd=21&ved=0CCkQFjAAOBQ&url=http%3A%2F%2Fwww.highfrequencyelectronics.com%2FArchives%2FMar11%2FHFE0311_Maloratsky.pdf&ei=1fq7Ufi8LMOriAf_soHoAw&usg=AFQjCNGIq8Zb5uDPTQj7I1ZzlxNh65C9_w&bvm=bv.47883778,d.aGc&cad=rja

See page 38; the general recommendation is for 4 - 5 line widths and there are some interesting comments on tapering the ground plane.

Also here;

http://www.google.com.au/url?sa=t&rct=j&q=&esrc=s&source=web&cd=36&ved=0CEUQFjAFOB4&url=http%3A%2F%2Fpeople.eecs.ku.edu%2F~callen%2F713%2F713_Gnd-Pwr_Planes-F11.ppt&ei=AQG8UaveD-PxiAfEvoGYBA&usg=AFQjCNGsRdC8-Tx0JxOLZbx2GYx9z4Yg-A&bvm=bv.47883778,d.aGc&cad=rja

are some comments on ground plane width; you could apply the maths described to decide the width at which the current has fallen to what you regard as a negligible amount.


Kerry VK2TIL.
8736 2013-06-15 10:19:02 Dave Miller Re: Microstrip to board edge desgin rule
Kerry,
Thank you for those interesting links.
Much food for thought. I was hoping for something definitive.
The portion on the current distribution is interesting and makes sense.

I guess this is an area where some experimentation and testing could be done.

I guess for now we will let the sleeping dogs lie and see how the PCB works once its made.
Thanks
Dave
VE7PKE

Sent from my iPhone

On 2013-06-14, at 23:09, "Kerry" <planningpower@iprimus.com.au> wrote:

> Good question; there is not much on this aspect of microstrip that I can find.
>
> The width of the ground plane is, in theory, infinite but the effect drops-off with distance from the centreline of the microstrip and, at some point, becomes negligible (a word that means different things to different people :) ).
>
> This "tapering" effect is analogous to skin-depth where one skin-depth is defined as the depth at which the current has fallen to about 0.37 times the current at the surface but current still flows at greater depths.
>
> I did find this;
>
> http://www.google.com.au/url?sa=t&rct=j&q=&esrc=s&source=web&cd=21&ved=0CCkQFjAAOBQ&url=http%3A%2F%2Fwww.highfrequencyelectronics.com%2FArchives%2FMar11%2FHFE0311_Maloratsky.pdf&ei=1fq7Ufi8LMOriAf_soHoAw&usg=AFQjCNGIq8Zb5uDPTQj7I1ZzlxNh65C9_w&bvm=bv.47883778,d.aGc&cad=rja
>
> See page 38; the general recommendation is for 4 - 5 line widths and there are some interesting comments on tapering the ground plane.
>
> Also here;
>
> http://www.google.com.au/url?sa=t&rct=j&q=&esrc=s&source=web&cd=36&ved=0CEUQFjAFOB4&url=http%3A%2F%2Fpeople.eecs.ku.edu%2F~callen%2F713%2F713_Gnd-Pwr_Planes-F11.ppt&ei=AQG8UaveD-PxiAfEvoGYBA&usg=AFQjCNGsRdC8-Tx0JxOLZbx2GYx9z4Yg-A&bvm=bv.47883778,d.aGc&cad=rja
>
> are some comments on ground plane width; you could apply the maths described to decide the width at which the current has fallen to what you regard as a negligible amount.
>
> Kerry VK2TIL.
>
>


[Non-text portions of this message have been removed]
8737 2013-06-16 14:01:08 Dave Hartman Re: Microstrip to board edge desgin rule
Don't know if this will help, it sounds like you're interested in
transitioning from stripline to connector or coax.

http://www.qsl.net/yo4hfu/Microstrip.html

but a Google search for stripline calculators brings up a lot of stuff.

Dave - AC2GL
8738 2013-06-16 15:05:42 Kerry Re: Microstrip to board edge desgin rule
I think the question put by Dave the OP was "How wide should dimension a in this diagram be?";

http://i39.tinypic.com/334olfd.jpg

Whilst most of the field lies between the trace and the ground plane, fringing fields extend further than that; "in theory" to infinity but there is a falling-off effect until, at some point, these fields can be discounted.

I think this point is not too far from the microstrip edge; 4 - 5 line widths was the only firm "rule - of - thumb" that I found.

I thought about the HP 805A slotted line I have in my little "museum" of interesting things;

http://i44.tinypic.com/68672t.jpg

This is composed of two flat faces about an inch apart with a centre conductor about 5/8" diameter. The fields look like this;

http://i39.tinypic.com/30xcqib.jpg

Intuitively I would have thought that there would be considerable leakage from this very wide slot but mathematics by those far cleverer than I (A New Type Of Slotted Line Section, WB Wholey et al) show that the slot width in the 805A is equivalent to a slot about 0.0006" wide in a conventional slotted line.

The obvious conclusion is that the fringing fields drop-away very quickly.

I did quite a bit of research as I was interested in the answer; I found very little in the extensive literature on stripline & microstrip that considers this matter.

Kerry VK2TIL.
8741 2013-06-17 14:03:34 augustinetez Re: Microstrip to board edge desgin rule
This is a quote from EMC information I have on hand. Assuming a 50 Ohm line on FR4 fibreglass, the track will be 2.8mm wide, so the distance to the edge would be ~9mm or ~30mm depending on how you interpret this paragraph.

"Transmission lines must not have any breaks, gaps, or splits in any of the planes they are routed over, as these cause sudden changes in Z0. They should also stay as far away as possible from any breaks, gaps, splits, or plane edges, by at least ten times their track's width. Low crosstalk requires spacing adjacent transmission lines by at least three times their track widths. A very critical or aggressive signal (e.g. a radio antenna connection) may benefit from using a symmetrical stripline with a row of closely spaced vias between its two 0V planes all along each side, `walling it off' from other tracks and creating a coaxial type of structure in the PCB."

You can access a pdf copy of the complete series of articles where the paragraph came from here:

http://www.humerboard.at/ftkl/Design_Techniques_For_%20EMC.pdf

Terry VK5TM
8743 2013-06-17 14:03:56 Dave Miller Re: Microstrip to board edge desgin rule
Kerry,
You are almost 100% correct in your statement.
In the application under discussion I was interested in a/2 ot the right
portion to the edge of the board. The direction to the left is ground plane
on bottom layer and ground plane infill on top and other circuitry.

Than you very much for your interest and finding that reference material.
So we will have to go with 4-5 line widths.

Thanks
Dave
VE7PKE

8745 2013-06-18 21:05:11 Dave Miller Re: Microstrip to board edge desgin rule
Terry,
That is a good collection. I have added the PDF to my reference material.
I have heard the author speak before at an EMC conference. He was very knowledgable.
Dr Clayton Paul also was awesome speaker. I had the pleasure to listen to him multiple times before he passed away. I cherish my autographed copy of his classic EMC book.

I guess 4 to 10 is what I will go with.

Thanks.

Dave

Sent from my iPad

On 2013-06-16, at 7:02 PM, "augustinetez" <vk5tm@internode.on.net> wrote:

> This is a quote from EMC information I have on hand. Assuming a 50 Ohm line on FR4 fibreglass, the track will be 2.8mm wide, so the distance to the edge would be ~9mm or ~30mm depending on how you interpret this paragraph.
>
> "Transmission lines must not have any breaks, gaps, or splits in any of the planes they are routed over, as these cause sudden changes in Z0. They should also stay as far away as possible from any breaks, gaps, splits, or plane edges, by at least ten times their track's width. Low crosstalk requires spacing adjacent transmission lines by at least three times their track widths. A very critical or aggressive signal (e.g. a radio antenna connection) may benefit from using a symmetrical stripline with a row of closely spaced vias between its two 0V planes all along each side, `walling it off' from other tracks and creating a coaxial type of structure in the PCB."
>
> You can access a pdf copy of the complete series of articles where the paragraph came from here:
>
> http://www.humerboard.at/ftkl/Design_Techniques_For_%20EMC.pdf
>
> Terry VK5TM
>
>


[Non-text portions of this message have been removed]