I would like to create a pcb, where the antenna patches, located on the top layer, are connected with vias to mcx ports (via in pad) on the bottom layer.
For the microstrip patch antennas i created a footprint with a bare copper area and placed a via inside the copper area in the pcb editor.
if you look at the blue(ish) bottom layer, you see a circular clearance cutout around the via. This means Kicad thinks the via (and the red circle on the top) belong to a different net. (Or to no net at all)
The first suspect here is the footprint itself. How is it made? Simply drawing graphics on a copper layer does not work well. You have to use pads, because otherwise KiCad is not able to attach a net (and thus tracks and via’s, etc) to it. You can create a complex pad by first drawing a normal pad, then select it and press [Ctrl + E] to edit the pad in “Pad Edit Mode”. In "Pad Edit Mode the extra graphics become part of the pad itself.
The best way to look at what’s really happening is if you create a small test project (with that footprint), zip it and upload it here. To be able to do that though you need at least 10 minutes of “viewing time” to prove to the (sometimes a bit annoying) bot that you are a human being.
A via needs copper on both sides. So maybe you can put a single tht pad footprint on the antenna.
Or better, include the hole into the antenna footprint.
Paul was faster than me…
Thank you @paulvdh and @pedro for the helpful responses! With the “Pad Edit Mode” i was able to fuse the antenna graphic with a Through Hole pad, located at the feed position. This is the result:
THT pads are very similar to via’s, but with a few differences.
THT pads are parts of footprints and act as connection points for wires, while via’s are placed directly on the PCB and only used to change layer.
THT pads have more abilities on other layers, such as the solder mask layer because they are meant to be soldered to.
During Gerber file creation there is an option to “tent” the via’s (cover them with solder mask) and this does not affect the THT pads.
Via’s are always round, while THT pads can be round, oval, (rounded) square, etc.
THT pads are a normal part of PCB design, there is no need to discuss them with your PCB manufacturer.
KiCad also has a thing called an Aperture Pad. Aperture pads do not exist on any copper layer, and thus do not have a pad number (you can’t connect a net to something that has no copper). Aperture pads can be used if you want to manipulate the other layers.
Both “aperture pads” and “THT pads as via’s” are used in default KiCad footprints. Look up any footprint with “Thermal” in their name to study how they are used. They are used a lot in big QFP’s with a big pad in the center. Such a pad can have many THT pad used as thermal vias in it, and then aperture pads are used to add small dabs of solder over the area of the pad.
I generally understand what you’re trying to do. However, at the frequency where you can use a patch antenna, the Via may not be a good idea. Just because you can put in a Via doesn’t mean it’s a good idea.
I don’t know nothing at all about patch antenna’s myself, but a simple picture search suggests that using a via as the connection point is relatively rare.
Usually the wire is just connected to the side, sometimes it’s connected more to the center with a small clearance cutout on the sides of the track.
Yes you are both right. If I had the choice i would rather use an inset feed. However, I need to have the coaxial cable connections at the bottom layer.
A good overview of the microstrip antenna feed methods can be found here: https://www.antenna-theory.com/antennas/patches/patch3.php.
I am trying to implement the “Coaxial Cable or Probe Feed”. I am rather inexperienced in antenna and pcb design, so I currently see no other way than to use a via to connect to the bottom layer.
Just for future reference: I ended up using a SMD-Type pad as an antenna (without solder paste), instead of a THT in the previous post and used a standard via again:
While paulvdh provided some good distinctions between a THT and a via, these distinctions are mostly for the designer. At the board fab house, plated THT holes and plated vias are handled exactly the same. While many vias have a smaller drill diameter than THT holes, there can be corner cases where this isn’t true. But the fab house usually doesn’t care. They only need to care about different drill diameters (and making sure that the hole diameter doesn’t violate the hole diameter to board thickness aspect ratio for reliable plating), and if they do any testing (not all do) where the holes in the solder-mask layers are.
Thank you! That should be everything I need, thank you to everyone for the help!
First reply I recently had a problem stitching vias to a 10mm track high current I found if I put a via in pcb editor out of the way then pressed e was then able to set net then select move and drag it any where on gnd plane
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.
