Announcement

Collapse
No announcement yet.

About strange computation of 120 ohm impedance

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

  • rhwalton
    replied
    Thank you Robert....that really cleared things up. I'm working in Altium 21 so things a just a tad different than your video. I did find the tool for measuring primitives.

    Leave a comment:


  • robertferanec
    replied
    Notice, I select "Measure primitives" ... that is the key. The dialog box then says "Distance between tracks".

    If I would select "Measure distance", then I would get the distance between the points I clicked.

    Leave a comment:


  • rhwalton
    replied
    Roger in your "Advanced PCB Layout Course" Lesson #4, around the 3:40 minute mark, it clearly shows you measureing the gap between 2 tracks and it apprears that you are clicking the center of the track and not the edge which would be normal for Altium unless you didn't use the snap and zoomed in on the edge of each track. The measurement you took and that showed on the pop window was center to center and not edge to edge. Did I misinterpret that? Also forgive my slow response but we have been under severe weather in our area.

    Leave a comment:


  • robertferanec
    replied
    gap is the space with no copper, so edge to edge.

    PS: please where exactly in lesson for?

    Leave a comment:


  • rhwalton
    replied
    Robert...can you clarify the meaning of measure the differential pair gap? and what is usually called out by the PCB Manufacturers? What I am trying to understand is the gap measured from track edge to edge or track center to center? and why one method is more accurate or important than the other.

    I found this guideline "The Anatomy of a Differential Pair" which suggest edge to edge but your lesson 4 stated center to center.

    https://www.ema-eda.com/sites/ema/fi...nfographic.pdf

    Last edited by rhwalton; 02-10-2021, 12:01 PM.

    Leave a comment:


  • robertferanec
    replied
    I would like to add, when you are designing track geometry for differential pairs (the track width and gap between tracks), very often you also need to follow single ended impedance requirements. For example, most tracks in differential pair will need to have 50OHM single ended impedance - that will help you to decide on the width of track which you need to use for your differential pair (so first you need to know track width for 50OHM and then you use this width as the track width of your tracks in differential pair). Based on the width and your stackup you will then calculate the gap between tracks for your specific differential pair impedance.

    PS: Theoretical calculator (such Altium calculator) will never give you the exact numbers, because theoretical calculator will not consider things what will happen during manufacturing process. For example, the thickness of prepreg in the real PCB may be smaller than thickness of prepreg material. (e.g. during PCB manufacturing, the prepreg will melt and it will flow between tracks on your PCB which makes the prepreg thickness smaller + during manufacturing the PCB is pressed under high pressure and that may also make thickness of prepreg smaller).

    So when I need to use impedance controlled tracks, I always follow the numbers which were sent to me by PCB manufacturer. I only use calculators to get approximate numbers.

    Leave a comment:


  • mulfycrowh
    replied
    I agree with what you're saying

    Leave a comment:


  • goncaloc
    replied
    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

    Leave a comment:


  • mulfycrowh
    replied
    OK but why AD19 is not able to find the right values?

    Leave a comment:


  • goncaloc
    replied
    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

    Leave a comment:


  • mulfycrowh
    replied
    Here what I've got for 120 Ohm impedance

    Leave a comment:


  • goncaloc
    replied
    double check your values, I get 120,25R

    Attached Files

    Leave a comment:


  • mulfycrowh
    replied
    But width remains wrong.

    Leave a comment:


  • mulfycrowh
    replied
    You are right!

    Leave a comment:


  • goncaloc
    replied
    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

    Leave a comment:

Working...
X