PCB Antenna Transmission Line - Polygon Error?

Am 22.09.2019 um 06:14 schrieb David Wyllie:

Hi,

 

Hoping some Eagle experts can help me understand either what I am doing wrong or what I need to do to get this completed. I am creating a PCB antenna using a coplanar waveguide in eagle and I cannot work out if I am doing it properly as I cannot get the isolation level correct around the transmission line.  In order to create the correct 50 Ohm impedance.

 

• I know I need a 0.74mm transmission line from the chip through my Pi network to the antenna

• I know I need an isolation of 0.11mm to the GND

• I will be using 1.6mm PCB with a dielectric constant of 4.6.

 

Please see the AppCad calculations below.

 

 

 

To build this layout in eagle I have researched online to understand I can try it several ways. But I am being checkmated each time I try.

 

First way: Use a Wire

If I use a wire to connect the airwire, I can define the width to be 0.74mm quite easily. However, if I do this it uses the DRC clearance level of 0.15mm. This 0.15 level will change my impedance. I can see the settings at 0.15mm under Edit -> Design Rules -> Clearance Tab is set at 0.15mm. If I change the grid to 0.11mm I can see that the distance to ground is 0.15mm using this method. Then I looked at setting this transmission line as a different Net Class under Edit -> Net Classes. But one cannot set the isolation around the wire. One can set the width of the wire in the net class but not the isolation.

 

 

Second Way:

 

So then I tried to create a polygon. I made the width 0.37 and worked my way between the antenna point below and the left hand edge of my Pi network (C15).I then continued between inductor L4 and C16. By setting the grid to 0.01 and being careful I can see that I can make a polygon exactly 0.74mm wide and give it a 0.11mm isolation in the settings.

 

 

 

 

 

however when I ratsnest it ignores the polygons and the isolation and fills it all in...

 

 

 

If I use Properties -> Convert To Wires, it once again uses the DRC at 0.15mm, which is checkmate, so I can't use that route.

 

Question One: How do I get the ratsnest to respect the polygons that I have built to be the transmission line to the antenna?

 

Question Two: The autoroute command will not complete unless I connect the air wires along the transmission line. Do I do this underneath the polygon?

 

Apologies if I am missing something simple and this is a silly question, however I am quite stumped by it and I've tried most every method  I can think of.

 

Best,

SteadyD

 

--

To view any images and attachments in this post, visit:

https://www.element14.com/community/message/281962

 

I cannot help much.

You should always tell us your eagle version.

Consider a polygon as an area with a fence. To get out you must change

to a different layer.

BTW. Auto router is not the best idea. It gives up if there is no

connection possible according its setting .

Polygons may have a name and a different RANK.

Check the Help for polygon and rank.

--

Mit freundlichen Grüßen / With best regards

Joern Paschedag

look at https://www.baldengineer.com/eagle-ground-plane-polygon-fills.html who has a good grasp on the subject. On the ohr hand https://electronics.stackexchange.com/questions/73868/eagle-digital-gnd-polygon-does-not-fill  explains a problem of not filling in a polygon I think. The part that caught my eye:

Looking at the clearance area around your pads, the problem is most likely the pad-to-wire clearance setting in your design rules. If the clearance (minimum distance) is set too high, the polygon place can't connect to the respective PIN. As a result, the polygon won't fill at all.

I can reproduce your problem just fine setting the highlighted value to something like 80 mil.

Hi,

Personally I'd use a normal trace route for this, rather than try to create a polygon for it. You can change the DRC setting to allow 0.11mm if your PCB factory supports this, because the point of the DRC is to indicate the technology limits of the PCB manufacturer. Or, another option is to ignore the slight difference, because it's unlikely that the calculation will be precise anyway, unless you're paying a lot for a special PCB. Or, you could increase the trace width slightly (e.g. to 1mm) and then the calculation will allow for greater clearance of about 0.15mm, which meets your design rules.

If you're using polygons, uncheck Orphans and uncheck Thermals settings. I can't help with the autoroute question, I don't usually use that (and especially not for an RF circuit).

Thank you Shabaz,

Some fiddling in AppCad and a slight increase in the transmission line width,  some tweaks to the DRC; and we are there.

Best,

SteadyD