IWR6843: iwr6843 pcb fabrication confusions

1) Our pcb fab said,galvanic effect at the junction between antenna and solder mask may affect antenna signal,if we insist on immersion silver,is galvanic a problem?

>> In the  immersion silver process silver oxide is expected if it's exposed to prolong period to the external environment, However this should not cause performance degradation for the mmWave application as silver oxide is also a good electrical conductor at mmWave frequencies. 

2)shengyi technology s1000 pcb fab recommended another stackup,L1-L2 is ro4835,L3-L6 is shengyi technology s1000(FR4).we are not sure if this stackup and FR4 material are available.And the thickness of layer copper is OK?

>> In the stackup base Cu thickness (while ordering material from Rogers) on the top side (Antenna side) should be 0.5Oz and bottom side is 1Oz,

1Oz is not recommended on the top side as antenna simulations are done with 0.5Oz Cu at mmWave application thin Cu is preferred on the Antenna layer, and material type should be RO4835LO PRO, as non-lo pro RO4835 materials are also available (Just to avoid incorrect ordering of material based on stackup) which are lossy at mmWave frequencies.  Top side of the Cu goes through two times plating process hence finished thickness should be less than 1.6mil and 2nd layer (gnd) of RO64835LOPRO goes through single plating process hence finished thickness should be 1.4mil.  

3) In the PROC073B fabnotes,PTH copper thickness is 20um_30um.There is no thickness about L1-L2 blind hole copper thickness.what is requirement of the blind hole. our pcb fab provide a design:PTH copper thickness average 25um,min 20um. blind hole copper thickness average 18um,min 15um.is this design OK?

>> Blind hole copper thickness average 18um,min 15um is ok. 

4) What is the requirement of copper thickness and tolerance about antenna

>> Explained above, Trace width tolerance is +/-1mil 

5.What is requirement of copper thickness of antenna,including base copper and finished copper?

>> Explained above point 2

6.L1-L2 PCB material Rogers 4835 4mil core1/1 Low Pro is OK? what are differences of H/H、1/1、H/1.

>> Design is developed with H/1 : This means half Oz Cu on the top side and 1Oz Cu on the bottom side of the RO4835LO PRO substrate.

If the above substrate is absolutely not available then next best alternative is H/H, i.e. Half Oz on top and half Oz on the bottom side. Thicker cu for the ground is better for thermal and better power integrity.  

7. our pcb fab said:whatever surface finish,L1-L2 blind via can not be filled? is this real? Will unfilled blind via  affect antenna signal?

>> Around the RF balls there are via on the pad to get the best S11 performance, If the via filling and surface plating is not done then there is a risk of solder paste getting sucked in to via holes during the re-flow process and causing poor solder joints.

8.Our pcb fab said if 50ohm antenna traces can not match 50ohm,can they adjust antenna trace width?Or according to the original size, do not control impedance.

>> Antenna traces should not be adjusted as trace width, air gap, via locations for grounded co-planar wave-guide (GCPW) based on 3D Electro magnetic simulation. Hence please use the design targets provided in the Altium design. If the fabricator 50 Ohm adjustments are planar they cannot guarantee 3D 50ohm for GCPW. Altering the trace width/Airgap from the design will cause degradation in the Antenna performance, hence not recommended. 

Target the trace width and air-gap according to design within +/-1 mil etching accuracy. 

Thanks and regards,

CHETHAN KUMAR Y.B.

11.and if we use Rogers 4835 4mil coreH/H Low Pro，In order to prevent PCB board warping, both sides need to be symmetrical. L5 and L6 base copper need to be 0.5oZ，is this OK？

>> For small size board warpage is not a problem, However if it's a concern it could be adjusted in other layers.

12.Can S1000 replace 370HR about FR4 material，attachment is S1000 datasheet S1000.pdf

We do not have experience in  S1000, But I have a concern on bonding with Rogers material. Has this been proven from the manufacturer on high volume production?  There seem to be high CTE (Coefficient of thermal expansion) difference between two materials. This need to be looked at. If the manufacturer has reliably built PCB on high volume then, it's ok. 

Thanks and regards,

CHETHAN KUMAR Y.B.

we find that in PROC073B fabnotes,dielectric of L2-L3 and L4-L5 not the same. I think these two should be the same thickness.

Why not the same?

If we adjust all to 5.67mil,is this OK?

>> There are high speed lines LVDS lines are present in the design, which needs controlled impedance for strip-line configuration to accommodate stackup has been adjusted as dielectrics are different on L1-L2 interface and L5-L6 interface. 

If you don't use LVDS interface then 5.67mil should be ok. 

Thanks and regards,

CHETHAN KUMAR Y.B. 

Hello,

   I have shared the link. 

Thanks and regards,

CHETHAN KUMAR Y.B.