Hi,
do you recommend a PCB supplier for 80 Ghz antennas?
It seems that not all support this frequency.
Thanks
Fred
This thread has been locked.
If you have a related question, please click the "Ask a related question" button in the top right corner. The newly created question will be automatically linked to this question.
Hi,
do you recommend a PCB supplier for 80 Ghz antennas?
It seems that not all support this frequency.
Thanks
Fred
2438.mmWave_hw_design_guide_rev_9.pdfHello,
The PCB design, has to meet tight tolerances 1mil, for dimensions and work with multiple laminate materials as shown in the stackup drawing.
Currently the PCB for the 80Ghz EVMs is fabricated by Streamline in Plano Texas.
PCB fabrication concerns from the RF perspective are covered in this section. This includes a discussion of CAD to CAM RF design documentation and how to evaluate PCB fabricators for RF fabrication quality. The goal here is to describe the key points to bring up and align on with a selected PCB fabricator to achieve first pass success when fabricating mmWave PCB.
Currently TI only supports two RF substrate stackups for mmWave sensor designs. These are Rogers RO3003 and Rogers RO4835 LoPro substrate designs presented in the mmWave HW Design Guide . RO3003 substrate is used on TI internal validation boards and is a higher RF performance (and higher cost) RF substrate than the RO4835 LoPro used on the BoosterPack EVM designs.
Designers should discuss with their PCB vendor the vendor’s experience with fabricating PCB with Rogers substrates. Rogers fabrication documentation covers material storage, material handling and material processing techniques. All of these recommendations must be followed to achieve consistent performance when utilizing these materials.
Rogers fabrication documentation:
Designers should discuss whether their PCB fabricator is taking delivery of copper-clad substrates directly from the RF substrate vendor or performing on-site plating of the substrates. Using the copper-clad substrates from the RF substrate vendor reduced variability in performance of the copper plating, therefore decreasing variability in the final RF design as well.
Sequential lamination of RF and non-RF substrate core and pre-preg material is typically required for completing RF designs such as the BoosterPack EVM. Designers should discuss with their PCB vendor the vendor’s experience and capabilities when fabricating mixed material sequential stackups. Different core and pre-preg materials typically have different curing requirements and procedures and may not always be compatible.
RF signal paths exhibit high sensitivity to small geometry changes such as:
• Substrate thickness
• Metal thickness
• Metal roughness
• Plating
• Via placement tolerance
• Etch tolerances (LDI vs. LPI masks)
• Air gap tolerances
• Solder-mask tolerance (LDI vs. LPI accuracy)
• Sequential stack-up layer registration
Substrate thickness directly determines performance of the RF structures. RO4835 LoPro and RO3003 substrates should maintain their designed thicknesses as received from Rogers. However, improper handling or fabrication steps can damage these substrates causing delamination and other adverse effects which will severely impair any RF structure performance.
Overall etch tolerances must be controlled so that the line widths, air gaps and planar antenna structures stay close to their designed dimensions. TI recommends using laser direct imaging (LDI) etch-mask over more common liquid photoimageable (LPI) etch-mask because LDI enables tighter tolerances fabrication. Reference the HW design guide
In the case of solder-mask in RF regions, like near the RF BGA, it is critical that the solder-mask registration and thickness must be tightly controlled. Solder-mask will have different dielectric properties compared to the RF substrate and the free-space surrounding the PCB. Because of this, changes in thickness or registration can have an effect on variability of RF performance PCB to PCB. TI recommends using LDI solder-mask over more common LPI solder-mask because LDI enables tighter tolerances fabrication. Reference the HW design guide .
Over and under plating of top-layer copper can result in phase and loss/reflection variations. TI mmWave BoosterPack designs use a 0.5 oz/inch^2 LoPro copper. Rolled copper may be used as well. RF designs cannot use electro-deposited (ED) copper since the variation in final thickness and roughness is too large. Immersion silver plating is used over RF sections of the board where solder-mask cannot be applied. Reference the HW design guide .
Via distances, for example, the microvia ground stitching surrounding the BGA and GCPW structures are critical to creating balanced ground return paths around these structures. A uniform offset in one axis may result in an imbalance in E and H-field distribution which will change the impedance of the structure.
Absolute tolerance limits on each dimension and placement can only be derived from margin studies using RF simulators and EM theory. The process involves sweeping various parameters, through a reasonable tolerance limit and determining how the parameter changes effects the performance of the structure. For example, designers can simulate with different air gaps, via placement distances, line widths and see the resulting change in GCPW impedance or antenna gain or directionality. Such studies are beyond the scope of this application note. we use a 1 mil tolerance from the Hardware Design guide table.
Designers are encouraged to clearly document the areas of the PCB that are RF design critical along with the intended design dimensions for each of these locations. Controlled impedance trace dimensions and stack-up thicknesses for high-speed digital signals are typically dictated and verified by a PCB fabricator. However, RF design dimensions should be dictated completely by the PCB designer and verified after fabrication.
In the case of these mmWave sensor designs the areas around the RF signal BGA footprints, the RF signal transmission-lines and the antennas must be carefully milled, drilled and etched. Ideally the tooling error must be constrained to zero-mean error around the designed dimension. Typical PCB fabrication error will result in a low variance skew in one direction of the tolerance window. PCB designers will need to discuss methods with their fabricator for bringing this skew as close as possible to the designed dimensions.
It is recommended that PCB designers explicitly ask for a small sample run of PCB to be used for process inspection purposes. Any problems meeting critical RF design dimensions can be dealt with before proceeding to larger volume production. This process can be repeated until the zero-mean error between fabricated and designed dimensions are achieved.
A report of critical RF design dimensions should be presented to the PCB fabricator part of the the PCB CAD and CAM board design documents and files. The PCB fabricator should be explicitly asked to verify what the expected tolerances are going to be for each of the critical dimensions.
Regards,
Joe Quintal
Dear Joe,
fantastic answer. Thank you very much for posting it!
How do you see a change of material from Rogers RO4835LoPro to RO4350?
It seems that RO4835 is almost impossile to source and PCB vendors keep telling me that RO4350 is almost as good as the one recommended.
Thanks,
Markus