Announcement

Collapse
No announcement yet.

Altium Impedance Calculator

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

  • Altium Impedance Calculator

    How good is the impedance calculator in Altium 21 if the parameters are entered from the board manufacturer?

  • #2
    If the fab shop is providing the stackup and trace/space widths you shouldn't need Altium's impedance calculator.

    Comment


    • #3
      Normally I would, but when dealing with JLCPCB, I have not been able to get anything for a 6 layer stack up. Specifically, I requested trace with on layer two and layer five if layer one and layer six are treated as the reference plane. I have yet to get anything back from them. There online calculator gives good for layer one or layer 6, but when selecting inner layer, it seems way off as if they where calculating from layer three to layer one as it shows two dielectrics which really was weird. What I did observe from their four layer board calculation and know ideal stack up is that for the prepreg ideal is 0.1 and in their calculator it appears as 0.0889. When I entered these into the Altium board stack up and examined the impedance, they both almost agreed. This is why I asked the question. What I observed from ideal to real was well within the margin of 10% error.

      Comment


      • #4
        Whenever I have compared fab nos of impedance with calculation nos, I have almost always found the difference to be less than 5 Ohms.
        I am not an expert though.

        Comment


        • #5
          I believe, Altium has improved the calculations, but I have not really investigated how accurate they are. However, I am very careful about everything what Altium calculates - they keep changing equations or they do not tell you what everything is included in the calculations and what is not (e.g. signal length, signal delay, etc), so I always rather use Saturn PCB Toolkit.

          From calculators, you may never get the same numbers as PCB manufacturer will tell you, but the numbers are not so different. So when I can't get numbers from a PCB manufacturer and I do not have access to expensive software like cadence or ads, then I just use Saturn PCB Toolkit to calculate impedance.

          Comment


          • #6
            Hi,
            I used the Altium calculator for a 10 layers board and compared the data sent by the fabricator.
            They were quite close in terms of trace impedance, width and spacing etc.

            Thank you.

            Comment


            • #7
              Related, what I'm curious about is how close to correct impedance can a designer get if they use the calculators and have the PCB manufactured without informing the fab shop of the controlled impedances. I often see on PCB fab notes that tolerances for impedance are +/-10%. This allows for a 20% variance, which seems enormous for a feature of the design that's intended to be controlled. I have a hunch that with that much allowable variance that simply calculating appropriate values for trace width and spaces, etc. should be enough to get me within +/-10% impedance without having to inform the fab shop that it's a controlled impedance design.

              robertferanec perhaps a topic for a video? If you do a few controlled impedance designs and shop them all out to a variety of fab shops without letting them know that they're controlled impedance designs? Then test all the PCBs you get back to see how close things get to desired values? For any one shop, a single design per week or something so that one design is never part of the same lot as another and so forth. What do you think? Can you test to see if declaring to the fab shop a design is controlled impedance worth the increased cost?

              Comment


              • #8
                Hi,
                I would always tell my fab house if I have any controlled impedance.
                As you said that tolerance are included while fabrication of the PCB, these fab house have to adjust several parameters to achieve that.
                Also they actually measure the impedance and submit you a report if requested.

                If you wanna confirm how good is the tool any of the two ways can be followed:
                1. Design a stackup and use the calculator for some impedance calculator. -> Go to some fabricator's websites like sierra circuit where they have their own calculator which they share online (After registration) and compare the results.

                2. Design and stackup in altium, For ex: 8 layers and impedance control of 100 ohms on layer 2 and 7 and ask your fabricator to suggest a stackup for same 8 layers and trace impedance of 100 ohms for layer 2 and 7 and compare the values.

                FYI, I followed 2nd option and values were quite similar.

                Thank you.

                Comment


                • #9
                  perhaps a topic for a video?
                  I do not have the tools to measure impedance. But it could be interesting to see how close the cheap PCB manufacturers would be with their impedances.

                  Comment


                  • #10
                    Originally posted by robertferanec View Post

                    I do not have the tools to measure impedance. But it could be interesting to see how close the cheap PCB manufacturers would be with their impedances.
                    But in previous videos, you have collaborated with people who have the test equipment for this. When you look at power delivery frequency response using a bode 100. I imagine a bode 100 could be used to show the impedance of PCB traces ¯\_(ツ)_/¯ Perhaps even plot the impedance characteristic over a range of frequencies?

                    Comment


                    • #11
                      Yes, other people could measure it ... just ... it is not always as simple as it looks in my videos e.g. many people are super busy and sometimes I need to wait several months to get 2 hours of their time.

                      Comment


                      • #12
                        Hi Folks,

                        Terrible what Altium does it in their impedance calculator. Since AD19, their has replaced the internal motor to SIMBEOR, but sometimes AD19, AD20 and AD21 calculates different results for the same situations up to 10% differences. A lot of bugs are/were in the backgorund (mathematic rounding bugs).
                        Today, I usually don't believe what Altium shows. But please inform me if it is being changed in the future.

                        About JLCPCB:
                        Their online calculator based on POLAR SI9000. The difference between published layer stack values and online tool come from parameteres from real live. The used shrinked thickness values are based on real measured values and informations are below.
                        Their matterial type at 4/6L is NP-155.
                        NP-155FTL_NP-155FR_NP-155FB.pdf (technolam.de)
                        The final prepeg thickness is depends on pressure and how many coppers remain in neirbour layers. That's why e.g. prepeg 2313 with 0.1mm (3.94mil) initial thickness has to calculated as 0.089mm (3.5mil). Usualy Remained Copper 70-80% is taken account.
                        Click image for larger version

Name:	NP-155FB.PNG
Views:	275
Size:	49.8 KB
ID:	17664

                        About Eurocircuits:
                        Their formulas are based on different sometimes non published algoorithms. They has made measurements and choiced the best. They has confirmed me, that the used formulas are very simple formulas. They are recommening to use 3th party calculators.

                        About Saturn PCB Toolkit (latest v8.05):
                        Take account, the internal used formulas sometimes don't equal on Conductor Impedance tab and on Differential pairs tab (e.g. microstrip Zo vs Edge Cpld Ext Zo). It could result 5 Ohm resistance.
                        Take a look the new Conductor Impedance tab Assymetric Stripline, where they are already enabling to select to internal used formula (Default, IPC-2141 and Wadell). The results are very differents (30R vs 55R)!

                        About online tools and official publications:
                        They are very different. The used formulas are based on different equations and there are wrong calculators, because of programmer mistakes!
                        But sometimes companies publishes wrong formulas, which are copy / paste by others. Do they do it directly?

                        - Fake Altium published IPC-2141 microstrip impedance formula: Impedance Calculations and PCB Stackup Design in Altium Designer
                        - An other Altium publication, but Wheeler’s equations for microstrip trace impedance is not correct: Clearing Up Trace Impedance Calculators and Formulas | Blog | Altium Designer


                        Final conclusion:
                        Sometimes PCB houses (e.g. JLCBCB, Eurocircuits) don't have calculator for specific layer stack combination, They say us, use POLAR, or other expensive tool. But we don't have it. We have Altium Designer with integrated SIMBEOR modul, which is much more expensive year by year. AD should be precise tool to give us results.

                        I hope this guide was usefull.

                        Attila

                        Comment


                        • #13
                          VUHA thank you Attila

                          Comment

                          Working...
                          X