Author Message
 Post subject: PCB antenna layout
PostPosted: 10 Jun 2017, 17:39 

Joined: 10 Jun 2017, 15:44
Posts: 8
I am trying to layout a meandering PCB antenna, according to Cypress's guidelines:

Basically, I'm trying to create a pattern with the following constraints:
  • A custom meandering copper shape with specific dimensions
  • Two pins on that shape (with no solder mask for either, where one connects to the top layer, and one connects by via to the bottom layer.

I've attached a pic from the above app note to show what I mean.

I've tried creating a pattern with a bunch of rectangles on the top layer that match the exact dimensions. Unfortunately, these create lots of DRC errors, as the copper is connected together or tied to any net.

What's a reasonable way to achieve this? And example PCB antenna designs?


You do not have the required permissions to view the files attached to this post.

 Post subject: Re: PCB antenna layout
PostPosted: 11 Jun 2017, 10:59 

Joined: 20 Jun 2015, 14:39
Posts: 943
Below you will find a DipTrace (v3.1) PCB file named "AN91445.dip" with the antenna you need. If you are using an older version of DipTrace, I can provide the ASCII file upon request. Here's how to place it into your board layout...

1) Launch the PCB Layout editor and open your board layout.
2) Open the antenna file named "AN91445.dip" in a second instance of the PCB Layout editor by double-clicking on it.
3) Select all of the antenna objects in the Design Area (Ctrl + A) and copy it to the clipboard (Ctrl + C). You will notice that all of the antenna objects are already grouped together.
4) Close the second instance of the PCB Layout editor containing the antenna.
5) In your board layout, right-click once in a blank part of the Design Area near the desired destination point for the antenna and choose Paste in the pop-up-menu.
6) With the antenna group still selected/highlighted, use the arrow keys to nudge it into the desired position on your board. (Change the grid size as needed for a more precise placement.) You can also rotate the antenna group if necessary using the [Space] bar.
7) To connect the antenna's ground plane, use the Place Ratline tool to drag a ratline between one of the antenna's Static Vias and a pad or Static Via on your board belonging to the desired Net. When a pop-up menu appears after the second mouse click, choose to merge the two nets. Be sure to double-check the Net name after the merge.
8) Repour all copper pours.
9) Resave your PCB file.

FYI: The antenna was created using Gerber files imported from the website link in the datasheet. Ground planes were replaced with copper pours, and Static Vias of the recommended hole size and spacing were added. All Static Vias and copper pours were assigned to the same Net. The lone Static Via connecting the end of the short antenna element to the bottom copper pour should be the only object the DRC flags (ignore it). When connecting to the antenna feed be sure to assign the antenna element to the same Net assigned to your transmission line (right-click on the element's outline and select Properties... in the pop-up menu).

Be sure to double-check all dimensions and let me know how everything works out.

p.s. If you would rather import a drawing file instead, I can provide a DXF file containing the outlines for the three ground planes and the main element.

You do not have the required permissions to view the files attached to this post.


 Post subject: Re: PCB antenna layout
PostPosted: 12 Jun 2017, 10:26 

Joined: 10 Jun 2017, 15:44
Posts: 8
Thank you - very helpful - gave me an idea of how I can do it in a pattern.

I've decided to use a pattern that consists of 3 pads: a square pad to connect the antenna feed line, a square through hole pad for the ground return, and a big polygon pad for the rest, that remains unconnected (but is really connected by coper to the other adjacent two pads).

Seem to work...

Display posts from previous:  Sort by  
Post new topic Reply to topic  [ 3 posts ] 

All times are UTC - 5 hours [ DST ]

Who is online

Users browsing this forum: No registered users and 4 guests

You cannot post new topics in this forum
You cannot reply to topics in this forum
You cannot edit your posts in this forum
You cannot delete your posts in this forum
You cannot post attachments in this forum

Search for:
Jump to:  
Powered by phpBB © 2000, 2002, 2005, 2007 phpBB Group