Hybrid PCB stack-up -- Rogers + FR4

[cjrathi]

Hi,

Initially We designed a board for 2-6 GHz band application. It used 4-Layer FR4 PCB material.
Its performance in 4-6 GHz band was very worst. It had very high dielectric losses at such high frequency.

Taking into account this consideration, now We have optimized the design.
We are planning to use hybrid stack-up ( Rogers R04003 8 mils + FR4).

Will this will reduce the dielectric losses at high frequency ?

Will this hybrid stack-up hamper the performance of board ?

Please help.

Thanks,
CR

 

[flanello]

This would reduce your losses if the Rogers has a ground plane and the HF signals are routed on the top of the Rogers board.

 

[Ow@i$]

the software that you are using will have option to tell about your material i.e. FR4 or Roger, simulate with both and check what difference it is creating...
why not using only Roger only why hybrid???

 

[cjrathi]

the software that you are using will have option to tell about your material i.e. FR4 or Roger, simulate with both and check what difference it is creating...
why not using only Roger only why hybrid???

The only reason for going with hybrid stack-up is the COST. The whole stack-up with Rogers will increase the cost I guess.

And anyways I think only Top Rogers will matter, not the below FR4 layers..

- - - Updated - - -

This would reduce your losses if the Rogers has a ground plane and the HF signals are routed on the top of the Rogers board.

Yeah. I know that and I have done exactly the same in the design. But I am concerned whether FR4 material below Rogers will affect the performance. What do you think ?

Thanks,
CR

 

[G0HZU]

I've made lots of designs using Rogers + FR4 stackups and I've always been advised to make the layer stack symmetrical or the board can warp. So a typical design might be 0.020" Rogers on layer 1 then a 4 layer FR4 core and then another 0.020" Rogers layer on the bottom layer. Some designs use up to 10 layers in the FR4 core.

If you go for 0.008" 4003 material then the microstrip width for 50R will be quite thin (0.018"?) and also the losses per inch could be up near 0.2dB/inch at 6GHz.

You will also have to use buried/blind vias in your PCB under any active devices that have a ground pad under them and this adds to the cost. Also, be wary of what PCB finish you specify as some plating finishes can introduce extra losses up in the GHz region especially on printed filters.

 

[cjrathi]

I've made lots of designs using Rogers + FR4 stackups and I've always been advised to make the layer stack symmetrical or the board can warp. So a typical design might be 0.020" Rogers on layer 1 then a 4 layer FR4 core and then another 0.020" Rogers layer on the bottom layer. Some designs use up to 10 layers in the FR4 core.

If you go for 0.008" 4003 material then the microstrip width for 50R will be quite thin (0.018"?) and also the losses per inch could be up near 0.2dB/inch at 6GHz.

You will also have to use buried/blind vias in your PCB under any active devices that have a ground pad under them and this adds to the cost. Also, be wary of what PCB finish you specify as some plating finishes can introduce extra losses up in the GHz region especially on printed filters.

Thanks GOHZU for your response. I have few queries, which I hope you'll clarify.

I want to use Rogers R04003 8 mils only, as less height will have less radiation. I have seen the loss of R04003 8 mils material. Its acceptable in our case.
Can't I use Rogers R04003 8 mils + FR4+FR4, giving overall 62 mils height ? Will it affect the performance of the circuit? Width of microstrip line is not an issue. We can adjust it as it comes.

What does PCB warping exactly mean ? Is it an issue with PCB fabrication ? Will such asymmetrical stack-up affect the performance ?

Thanks,
CR

 

[G0HZU]

I don't know what your design requirements are so I can't say if your layer stack is the ideal choice or not. Normally, I would choose 0.020" Rogers 4003 up at several GHz because the metal losses are lower than for 0.008".

Also, I don't know how big your PCB is. Normally, I work alongside a dedicated PCB designer who lays out a PCB for my RF design under my supervision. The PCB designer also talks to the PCB manufacturer and takes advice about choosing the best layer stack. Also they can advise me as to the issues with warping. Having an asymmetric layer stack on a large PCB is a risk for PCB warping and so is having an imbalance in the copper distribution (per layer) after etching.

So often the layer stack can change part way through a design due to feedback from either the PCB designer or the PCB manufacturer. The manufacturer can advise about cost implications for buried/blind vias etc.

Will such asymmetrical stack-up affect the performance ?

I think it just affects the risk of warping especially during solder reflow. But you really need to discuss your design with the PCB manufacturer to assess the risks of warping. If your board isn't very big then it might be OK

Hope this is useful to you.

 

[cjrathi]

I don't know what your design requirements are so I can't say if your layer stack is the ideal choice or not. Normally, I would choose 0.020" Rogers 4003 up at several GHz because the metal losses are lower than for 0.008".

Also, I don't know how big your PCB is. Normally, I work alongside a dedicated PCB designer who lays out a PCB for my RF design under my supervision. The PCB designer also talks to the PCB manufacturer and takes advice about choosing the best layer stack. Also they can advise me as to the issues with warping. Having an asymmetric layer stack on a large PCB is a risk for PCB warping and so is having an imbalance in the copper distribution (per layer) after etching.

So often the layer stack can change part way through a design due to feedback from either the PCB designer or the PCB manufacturer. The manufacturer can advise about cost implications for buried/blind vias etc.


I think it just affects the risk of warping especially during solder reflow. But you really need to discuss your design with the PCB manufacturer to assess the risks of warping. If your board isn't very big then it might be OK

Hope this is useful to you.

My RF board size is very small. It's 38 mm X 22 mm. SO I guess it will not be a problem. Still I'll confirm this from the manufacturer.

Thanks,
CR

 

[tony_lth]

It should hae no problem, I had designed RO substrate with two layers FR4, no problem. My PCB size is bigger than 100mm, no problem on warping. Maybe because my component are at least 0402 size. If your PCB has some eMMC, it may need consideration.

 

[cjrathi]

It should hae no problem, I had designed RO substrate with two layers FR4, no problem. My PCB size is bigger than 100mm, no problem on warping. Maybe because my component are at least 0402 size. If your PCB has some eMMC, it may need consideration.

Thanks Tony,

No eMMC are there on the PCB. It just has three QFN package ICs, two SMA connectors and few 0402/0201 package discrete components.

So, should I go ahead with this stack-up ?