No announcement yet.

Which dielectric material is the best to use in 2.4 GHZ RF

  • Filter
  • Time
  • Show
Clear All
new posts

  • Which dielectric material is the best to use in 2.4 GHZ RF

    I have a 4 layer RF design that includes 50 mhz and 2.4 ghz RF frequencies and I want to choose suitable dielectric material for that frequencies what should I consider while choosing the material?
    Isola® 370HR or RO4350B, which is the best to use in 2.4 GHZ?

  • #2
    I don't have a lot of experience in RF, but in high speed routing it depends on your track length. The longer the tracks, the lower your loss tangent needs to be. Does that apply to RF?

    ITEQ has some good materials but it depends on which brands your manufacturer has access to. They should be able to recommend something if you ask specifically for low loss tangent. Assuming I'm right about what you need for RF.

    Something you should consider though is the dielectric constant / permittivity. I'm guessing you have impedance requirements so you'll need to make sure the permittivity in combination with your layer stack can give you the impedances you need.

    Kind regards,


    • #3
      DanR Thank you for your quick responce. I have not long trace and I dont know the importance of loss tangent in RF circuit but I will search for it and as you recommend I will ask specifically for low loss tangent.
      Yes I have 50ohm impedance requirements but I think Altium sort it out for me in layer stack manager when I write the Dk , Df and thickness of the material but I have no idea about the relation between permittivity and impedance requirements. Is it something changeable for each impedance profile? or must be changed for each impedance profile?


      • #4
        Only if you need to care about loss tangent. High grade materials are expensive.

        Dk is dielectric constant, also known as permittivity (Er).
        ​Df is loss tangent.

        ​​​​​Both affect the impedance, along with track width, clearance and copper thickness and dielectric thickness.

        Don't be tricked be the dielectrics datasheet either. It will provide a dielectric constant at a certain thickness but it changes for each layer. e.g. if you have a core at L1-L2 and another at L3-L4, they will have a different dielectric constant to the prepreg at L2-L3. Resin density also affects the dielectric constant, not just thickness which is probably why prepreg and cores of the same thickness have different properties. Even stacking prepreg layers in a HDI design can result in a different dielectric constant than the previously applied layers. I need to confirm this, but I think this is either related to the copper pours or the way the prepregs are joined. All of this needs to be accounted for in high speed design.

        In RF, my best guess is that you mostly care about maintaining impedance and avoiding losses along the tracks length.

        Also, don't let your ground pours get too close to your impedance controlled tracks. They may behave like coplanar tracks which gave a different impedance. Unless you want coplanar. It's just something to be aware of.

        Last edited by DanR; 05-04-2021, 10:34 AM.


        • #5
          First of all thank you for your explanations. If Dk changes for each layer and it is not possible to understand the changed value of material's Dk , the impedance profile that Altium measure for specific Dk is not reliable.

          Yes maintaining impedance and avoiding losses for good signal integrity is my priority and I will pay attention to the subject about the measure between the ground pour and high frequency trace.

          Can you make suggestions on the placement of the Core and prepreg layers and their appropriate thickness values? Most probably I will use RO4350B (by a comparing Df,Dk and thicknes as you suggested ) as a dielectric material, Can I use the same material for core and prepreg ? On datasheet, there are various thicknesses available to choose, As I know Core layer should be thicker than prepreg layer Can I use the thicker RO4350B material as a Core layer ?

          Attached Files


          • #6
            In your screenshot, you've got a Dk of 3.48 for both core and prepreg at vastly different thicknesses. It should be different.

            Altium 20 and 21 are actually very close to reality. You just need to give it the right information for the calculations. I use Saturn PCB Calculator to double check and they're normally within ±0.1Ω. This is verified again by the fabricator. Mine uses one of the Polar products for that.
            When I get to work I might be able to take a screenshot for you.

            You can have the same material for core and prepreg. I'm not sure if you have to, but I've never seen a board that uses different materials. Doesn't mean they can't though. I would use different thicknesses but where possible I try to reduce the number of unique sizes. If a board has 1080 and 106 prepregs and 2116 cores, there is benefit in changing 1080 and 106 to the same size. Unless your design actually needs both. In a HDI board, you can end up with a different prepreg size for the HDI layers.

            With cores and prepregs it's usually best to let your fabricator decide that unless you need that level of control. For my last board, I wanted to control it because I wanted to be able to easily add more layers at any time while reusing existing impedance profiles, without having to go through importance profile design again. I cared more about my deadline which way around the cores and prepregs were since both were very thin anyway. Eventually I think we agreed to end the centre board on a core before the HDI layers started.

            With 4 layers there's only 2 choices anyway. You can have a single core in the middle sandwiched by prepregs, or 2 cores with a prepreg between them. The fabricators I've used seem to prefer the latter on boards with more than 4 layers. My best guess is that it involves less lamination steps. Reducing the number of steps in general results in a cheaper and easier board. With 4 layers I've seen it done the other way around with a very thick core in relation to the prepregs. Or sometimes prepregs are stacked in the middle to make up the thickness.

            If you're using a fabricator that mass produces random boards like PCBWay, PCBCart, etc, it might be a good idea to look up their standard layer stacks on their website and use them. This way your boards can be panalised with other orders to bring down the price and lead time. However, if your quantity/size is enough to fill up the panels, you don't need to care about the standard layer stacks. I typically ignore the standard stacks unless it's for a quick adaptor or something. And I normally use fabricators that don't list standard stacks.

            Last edited by DanR; 05-02-2021, 08:46 PM.


            • #7
              I think I might be overcomplicating things for you.
              For a 4 layer board with 50Ω impedance you should be able to go straight to the fabricator. They would normally come up with a stack that meets your impedance and total thickness requirements so that you can order your boards through them.
              I'd still ask for the parameters to put into Altium or Saturn to check their stack.

              If you need or want to look into more advance layer stack design then that's great. But I don't want to waste your time either.
              Even when I'm designing my own stacks, they still go through the fabricator for review.
              Last edited by DanR; 05-02-2021, 08:47 PM.


              • #8
                DanR Thank you for the precious imformation you have given me. First I will talk with my fabricator and require the parameters for Altium or Saturn. it will be much easy and time saving for me. Also May I ask a example Altium layer stack manager screenshot to examine while waiting the fabricator's answer.


                • #9
                  Yeh sorry about that. I didn't have much time today. I'll try post the screenshots tomorrow.


                  • #10
                    Hi Sukru,

                    In this screenshot, I set Altium and Saturn with the same parameters and you can see that they almost agree. Saturn reports 48.8226Ω and Altium reports 50Ω.
                    The reason Altium has a clean value, is because I used Altium's calculator to get the correct width and then transferred it to Saturn to compare.
                    The same can be done with differential pairs and coplanar single ended.

                    In all honesty, Altium is more powerful because, not only can it calculate for coplanar edge coupled pairs, it can also consider more parameters.
                    Although, I'll admit, Altium is much harder to set up.

                    The red arrows indicate parameters you will have to set in order to make both calculators give you the same (close enough) result.
                    However purple arrows indicate things you may need to consider that Saturn can't help you with. I'll show you that in the next screenshot.
                    Attached Files


                    • #11
                      In this screenshot, I have set all those extra fields.

                      I set the etch factor to 0.2 which gave me a different width for the track side furthest from the dielectric it is etched on.
                      I usually calculate etch factor from the transmission/impedance profiles the fabricator provides. They usually list a top and bottom track width.

                      I also enabled the checkbox for Altium to consider the solder mask, which set to have a dielectric constant of 4 in the layers section. This will come from your fabricator or datasheet, but fabricators don't normally like to provide this information because mask brands change all the time. It doesn't have much of an affect anyway.

                      I then set the mask thickness to 50.8µ in general, and 30.48µm above the tracks. The former is linked to the material thickness. I made these numbers up but they were near this for my last board. Having a different thickness for the top of the track has a minimal effect.

                      I set Altium to calculate the track width closest to the dielectric material, which produced 100.44µm (3.95mil) to get the same impedance that 126.59µm (4.98mil) produced with the previous settings. 126.59µm with the new settings produces 45.29Ω which, while within 10% of the target, doesn't leave any room for fabrication tolerance.

                      However, Altium doesn't make it easy to consider frequency. You can run simulations, define rules for it, define more specific material properties (if you enable them). I'm not sure how that will go.
                      This doesn't matter too much though because frequencies between 500MHz and 2.4GHz don't have much affect on 50Ω single ended impedance. If you need other profiles, then maybe it's worth a look. I'll show you in the next screenshot.
                      Attached Files
                      Last edited by DanR; 05-04-2021, 09:07 AM.


                      • #12
                        With the same settings as that second screenshot, I took another one of Saturn side by side.
                        On the left, you can see the calculation for 500MHz.
                        On the right, I changed my mind about 2.4GHz and went with 3GHz to show a larger difference.

                        500MHz was 55.5074Ω
                        3GHz was at 55.5210Ω

                        The difference is insignificant.

                        I didn't show you stripline or differential signals, but the idea behind them is similar to the microstrip signals in these screenshots.
                        Attached Files


                        • #13
                          Hi DanR I am grateful for all the information you provided. These informations were very useful for me and saved me a lot of time. Thank you very much.