PCB antenna layout

Making PCB Layouts, Manual routing, Auto-routing, Copper pouring, Updating from Schematic, Manufacturing Output
Post Reply
Message
Author
bri
Posts: 8
Joined: 10 Jun 2017, 15:44

PCB antenna layout

#1 Post by bri » 10 Jun 2017, 17:39

I am trying to layout a meandering PCB antenna, according to Cypress's guidelines:

http://www.cypress.com/file/136236/download

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?

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

Tomg
Expert
Posts: 1355
Joined: 20 Jun 2015, 14:39

Re: PCB antenna layout

#2 Post by Tomg » 11 Jun 2017, 10:59

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.
Tom

bri
Posts: 8
Joined: 10 Jun 2017, 15:44

Re: PCB antenna layout

#3 Post by bri » 12 Jun 2017, 10:26

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...

Antonio
Posts: 5
Joined: 27 Mar 2018, 10:52

Re: PCB antenna layout

#4 Post by Antonio » 11 Sep 2019, 10:23

Hi Tomg,
Do you know a Dip file for a 900MHz antenna like the attached one?
Antenna 900MHz.png
You do not have the required permissions to view the files attached to this post.

Antonio
Posts: 5
Joined: 27 Mar 2018, 10:52

Re: PCB antenna layout

#5 Post by Antonio » 11 Sep 2019, 14:24

Solved.
Imported Gerber File from manufacturer.

Tomg
Expert
Posts: 1355
Joined: 20 Jun 2015, 14:39

Re: PCB antenna layout

#6 Post by Tomg » 12 Sep 2019, 08:57

I have created a pattern file if you're interested in making a component out of it. Just let me know and I'll post it here along with a set of instructions.
Tom

Antonio
Posts: 5
Joined: 27 Mar 2018, 10:52

Re: PCB antenna layout

#7 Post by Antonio » 13 Sep 2019, 09:40

Hi Tomg,
I am interested in the pattern you created. Pls post it with instructions.
Tks a lot.

Tomg
Expert
Posts: 1355
Joined: 20 Jun 2015, 14:39

Re: PCB antenna layout

#8 Post by Tomg » 13 Sep 2019, 10:08

Adding the antenna pattern to an existing custom pattern library

1) Copy the pattern library file named "antenna.lib" (attached below) to your desktop.
2) Launch the Pattern Editor, choose "Other Libraries" in the Current Library Group selection panel (left side of display), in the main menu click on "Library" and then select "Open..." in the drop-down menu to bring up the Open dialog window.
3) In the Open dialog window search for and select/highlight the new pattern library file named "antenna.lib" (now located on your desktop) and click on the [Open] button to add it to the library list.
4) Now choose "User Patterns" in the Current Library Group selection panel and select/highlight the desired destination library.
5) Click on the Pattern Tools panel and select "Insert Patterns from Another Library..." in the fly-out menu to bring up the Insert Patterns dialog window.

6) In the Insert Patterns dialog window choose "Other Libraries" in the Libraries drop-list, select/highlight the library named "antenna", make sure its one-and-only pattern named "900MHz" is selected/highlighted and click on the [Insert] button. The new pattern's name should now be displayed in the patterns list just below the Pattern Tools panel on the left side of the screen.
7) Resave your newly-supplemented destination library (Ctrl + S).
8) Choose "Other Libraries" in the Current Library Group selection panel, left-click on the library named "antenna" to select/highlight it, then right-click on it and choose Remove "antenna" Library from "Other Libraries" in the drop-down menu.
9) Choose "User Patterns" in the Current Library Group selection panel and select/highlight any one of its libraries to release DipTrace's hold on the desktop file.
10) Delete the file named "antenna.lib" from your desktop.

Be sure to double-check all dimensions for any mistakes I may have made. The pattern has been designed with the first coordinate point centered and slightly inset upward from the bottom edge to facilitate a logical trace connection location. A Route Keepout area has been added on the top side to prevent intrusions by other copper objects. Top Solder Mask has been set to "Tented" and Top Paste Mask has been set to "No Solder". This antenna pattern can be attached to a one-pin antenna component (not included here) of your own creation using the Component Editor (see example below). Once the component with its newly-attached pattern has been saved in a custom component library, it can be used in any schematic and/or PCB layout.
ce.jpg
antenna.lib
You do not have the required permissions to view the files attached to this post.
Tom

Post Reply