Announcement

Collapse
No announcement yet.

About strange computation of 120 ohm impedance

Collapse
X
 
  • Filter
  • Time
  • Show
Clear All
new posts

  • About strange computation of 120 ohm impedance

    Hi everyone,

    I am using AD 19.
    My stackup has 4 standard layers.
    I would like to add 120 ohm tracks.
    Here attached the result.
    I am little bit surprised by the result: 0.018 mm is very small.
    I guess an error.
    Any idea?


  • #2
    For controlled impedance, if the built in trace width calculator calculates that the traces need to be incredibly thin, the you need to change something else in the design, like the dielectric material or the dielectric thickness. Perhaps try sharing the entire layer stackup, not just the impedance calculation portion?

    Comment


    • #3
      I tried to enter the attached stackup from my manufacturer.
      Now it is no more possible to reach 50 Ohm impedance...

      Any idea maybe?
      Thanks a lot.

      Comment


      • #4
        Hi Mulfycrowh

        AD19 does no support multiple Dielectric between copper layers, remove one of the prepregs and change de other to 180um
        You should have a 300um width for 50R

        Comment


        • #5
          Seems OK with 50 Ohm impedance but always getting a very small track for 120 Ohm.
          I should have something like 0.12 mm.

          Comment


          • #6
            I don't think you will be able to have both 50R and 120R on the same layer
            To increase the necessary width of a track you will have to increase the thickness of the prepreg, so when you have 0.12mm for the 120R your 50R will be so wide it won't be practical.


            Comment


            • #7
              My manufacturer made the computation for both impedances with the stackup I shared.

              Comment


              • #8
                I see...
                The thing is, your 50R are single ended and your 120R are differential and that makes a world of difference.

                In altium when calculating your impedances don't forget to set the correct type, single ended or differential


                Attached Files

                Comment


                • #9
                  You are right!

                  Comment


                  • #10
                    But width remains wrong.

                    Comment


                    • #11
                      double check your values, I get 120,25R

                      Attached Files

                      Comment


                      • #12
                        Here what I've got for 120 Ohm impedance

                        Comment


                        • #13
                          You will need to select the layer ( either Top or Bottom ) and the properties will show up, as you already have the values you just need to insert the values on the right place

                          Comment


                          • #14
                            OK but why AD19 is not able to find the right values?

                            Comment


                            • #15
                              The values AD19 is giving you are right, they are values that will solve the equations needed for this calculations, the thing is they are not the only ones.

                              You can adjust both width and separation to meet your specifications.

                              Lets say your manufacturer couldn't make track thin as 140um, and it needed to be 200um, in this case you could play with the gap to get your impedance

                              Comment

                              Working...
                              X