Announcement

Collapse
No announcement yet.

Altium right method to design a BGA daughter board with pads on the bottom side?

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

  • Altium right method to design a BGA daughter board with pads on the bottom side?

    I've a BGA component with 1.0mm pitch and 204pins. I want to create a PCB daughter board so that 90% of the total BGA footprint pads has to go to the bottom side and appear as pads. So that will allow the daughter board to place it on the main board push contacts connector.
    I mean when BGA is placed on the top the bottom side should something like shown in the left image below . Thru via or spaces in between the pads are not allowed in this pcb.
    Edit: I've found that Via-In-Pads is a working solution,something like shown in right image below, how true it is?. Can I be able to automate fanout with Via-In-Pads?. Please guide me.

  • #2
    Yes, you should be able to use VIA in PAD. You just need to ask PCB manufacturer to fill up the holes in the through hole VIAs.

    Comment


    • #3
      Originally posted by robertferanec View Post
      Yes, you should be able to use VIA in PAD. You just need to ask PCB manufacturer to fill up the holes in the through hole VIAs.

      Hi Robert,

      Thanks again for the reply!

      Yes, I agree VIA in PAD is good solution. But, here as per the project requirements I'm not allowed to use thru hole VIAs, instead buried and blind are accepted.However, I'm interested to know how to use the Altium's Fanout option to automate VIA In PADs for 127pin BGA chip. Could you please guide me.

      Tnx

      Comment


      • #4
        I do not use automated fanout. I simply use Copy&Paste to do any kind of fanout I need. Just create it once, copy it multiple times e.g. once you have the whole row, just copy the whole row ... it will be quick.

        PS: I am not sure if I would connect power pins through microvias. I would maybe rather use through hole VIAs placed between the PADs.

        Comment


        • #5
          Originally posted by robertferanec View Post
          I do not use automated fanout. I simply use Copy&Paste to do any kind of fanout I need. Just create it once, copy it multiple times e.g. once you have the whole row, just copy the whole row ... it will be quick.

          PS: I am not sure if I would connect power pins through microvias. I would maybe rather use through hole VIAs placed between the PADs.

          Robert,

          I did try copy and paste before and I truly agree its fast and easy method. But the design I'm trying to do now is using the 6xTFBGA chips (see attached datasheet) and want to have all the HV pins connected to PADs on the bottom side without having thru holes or traces on bottom side. I am ok to use VIA-In-PADs, Micro VIAs and Blind VIAs.

          At the same time I noted your point on Power pins where I will be using standard blind VIAs instead of Micro VIAs.

          Could you please throw some light on me and guide me how to use copy and paste technique for such design.

          Thanks
          Attached Files
          Last edited by iluvu; 06-19-2017, 12:02 PM. Reason: Attachment

          Comment


          • #6
            Nothing special. Copy & Paste:
            1) On one pin, create the kind of fanout you would like to have e.g. uVIA + track + Buried VIA + Track + uVIA
            2) Select the uVIA, press CTRL and hold it down and select all the other elements (track + Buried VIA + Track + uVIA)
            3) CTRL+C and click on the pad where this fanout is connected
            4) CTRL + V and click on the pad where you would like to place it (if you need, press spacebar to rotate)
            5) Once you place more fanouts (e.g. whole row), copy them all. Press CTRL + C and CTRL+V place next row.

            Comment


            • #7
              Originally posted by robertferanec View Post
              Nothing special. Copy & Paste:
              1) On one pin, create the kind of fanout you would like to have e.g. uVIA + track + Buried VIA + Track + uVIA
              2) Select the uVIA, press CTRL and hold it down and select all the other elements (track + Buried VIA + Track + uVIA)
              3) CTRL+C and click on the pad where this fanout is connected
              4) CTRL + V and click on the pad where you would like to place it (if you need, press spacebar to rotate)
              5) Once you place more fanouts (e.g. whole row), copy them all. Press CTRL + C and CTRL+V place next row.

              Robert, for some reasons the copy & paste is not working when I try to copy the pins within the component from PCB layout. Then I tried to explode the components to free primitives which allowed me to copy and paste. I'm quite unsure of this option because If I explode and copy all the pins/pads with NETs then later when I had to undo the explode there is no option.

              Click image for larger version

Name:	Capture_456_ 21-06-2017.PNG
Views:	1
Size:	45.9 KB
ID:	1169

              Any suggestions?.

              Comment


              • #8
                You do not need to copy the pads - just the vias and tracks.

                Comment


                • #9
                  Originally posted by robertferanec View Post
                  You do not need to copy the pads - just the vias and tracks.

                  I see, then again I've to place the PADs seperately on bottom side and connect them?.

                  Comment


                  • #10
                    If I would do it, I would probably place two same footprints on the PCB - one on the top, one on the bottom. I would connect them in schematic and then do the layout. But I am not sure if I understand exactly what you are trying to do

                    Comment


                    • #11
                      Originally posted by robertferanec View Post
                      If I would do it, I would probably place two same footprints on the PCB - one on the top, one on the bottom. I would connect them in schematic and then do the layout. But I am not sure if I understand exactly what you are trying to do

                      Hi Robert,

                      Thanks for the suggestion. To be more precise this board is a daughter board which goes on to the main PCB and I can't really explain more about the main board as its not under my control. But technically what I know is these two boards will be placed in some kind of hard frictional environment and for these reasons the thru hole and bottom traces are avoided and bottom PADs has to be double the size of the chip PADs.

                      Anyway, I will consider your suggestions and use my experience as per the requirements and continue to work towards the goal. Thank you very much for your time Highly Appreciated!!!. If I get more questions then I'll get back to you later
                      Last edited by iluvu; 06-21-2017, 08:02 AM. Reason: typo error

                      Comment

                      Working...
                      X