CC2531芯片，天线选择问题。

你好:

     CC2531芯片，06mm的FR4，使用AN043天线，除去天线板子尺寸11*19mm。通信距离短，刚入门做zigbee节点， 能推荐一个更适合的天线或者，天线调整办法吗？

先用频谱仪分析下发射功率，频偏，用网络分析仪分析下阻抗匹配，TI的参考设计如果完全参照，距离还是不错的。距离短不是换换天线就能解决的。

如下是一些射频设计的考量：

Below is some additional notes when you are copying TI Reference design.

Understand the PCB board properties

–        PCB stack-up

–        PCB board dielectric properties (dielectric constant and loss tangent).

–        TI reference designs include a document describing above properties Readme.txt

The checklist below provides important RF PCB design considerations to be followed

1. Verify the stack-up matches the reference design. If the design is a 4-layer PCB; verify that ground plane is layer two right below top/component side.
2. Changing the layer spacing/stack-up will affect the matching in the RF signal path and should be carefully accounted for as explained in AN068
3. Ensure that you follow the datasheet layout recommendation unique to the part (CCXXXX).
4.  0603(mills) discrete parts are not recommended because of size and parasitic values.
5. Verify that bypassing/decoupling capacitors are as close as possible to the power supply pins that they are meant to bypass/decouple.
6. Ensure each decoupling capacitor only decouples the specific pins recommended on the reference design and that the capacitor is correct value and type.
7. Ensure that decoupling is done pin<>capacitor<>via.

1. Verify that the ground plane matches the reference design.  There should be a solid ground plane below the device and the RF path. 
2. Verify that RF signal path matches the reference design as closely as possible. Components should be arranged in a very similar way and oriented the same as the reference design.
3. The crystal oscillator should be as close as possible to the oscillator pins of the part. Long lines to the oscillator should be avoided if possible.
4. Verify that the top ground planes are stitched to the ground plane layer and bottom layer with many vias around the RF signal path.  Compare to the reference design.  Vias on the rest of the board should be no more than l/10 apart.
5. If the part has differential output, ensure that the traces in the differential section and differential section are symmetrical as in the reference design.
6. If the design uses a battery (such as a coin cell), the battery will act as a ground plane and should therefore not be placed under the antenna.
7. If the reference design specifies using T-Lines (Transmission Lines), it is very critical to ensure that the T-Lines match the reference design exactly.

1. Verify that the under-the-device power pad layout is correct. The solder pads and mask should match and the opening size should ensure correct amount of paste. Vias should be the correct number and masked/tented to ensure that they don’t suck up all the solder, leaving none to solder the chip to pad. (Refer to the datasheet for the recommended layout for the corresponding part)
2. The board should specify impedance controlled traces. That is, the layer spacing and FR4 permittivity should be controlled and known.

Important considerations for Antennas

1. If using an antenna from a TI reference design, be sure to copy the design exactly as drawn and check if the stack-up in the reference design matches your stack-up.
2. Changes to feed line length of antenna will change input impedance match.
3. PCB and chip antennas should not have any ground plane under them.
4. Any metal in close proximity, plastic enclosure, and human body will change the antennas input impedance and resonance frequency, which must be considered in the design.
5. For multiple antenna on same board, use antenna polarization and directivity to isolate.
6. For chip antennas verify that the spacing from and orientation with respect to the ground plane is correct as specified in their datasheet.