Forum Rule: Always post complete source code & details to reproduce any issue!
Results 1 to 5 of 5

Thread: Trace Width for MK64FX512VMD12

  1. #1
    Senior Member
    Join Date
    Oct 2014
    Posts
    167

    Trace Width for MK64FX512VMD12

    Just wondering what you may consider a trace width for the above. Is .1mm ok to trace around the IC? or is it too thin.
    All others will be 2x's the width once done.

  2. #2
    Senior Member
    Join Date
    Dec 2014
    Posts
    306
    It all comes down to trace impedance, which in turn is based on a variety of factors including:

    Target board copper thickness (2 oz/ft is the 'standard', however 1 oz/ft is commonly available and cheaper, however will increase trace resistance)
    Board layer and layer stack-up. Is it a two layer board?
    Trace length
    Required current capacity

    and onwards. IPC-2221 calculators such as http://www.4pcb.com/trace-width-calculator.html will give you a good idea. You will also need to check with your intended manufacturer their minimum requirements as these will differ. For instance ITead have a minimum requirement of 0.15mm (http://support.iteadstudio.com/suppo...b-capabilities)

  3. #3
    Senior Member
    Join Date
    Oct 2014
    Posts
    167
    I just sent the Gerbers out to see. Not to large of a board and the length of the longest trace should be ok. I had a hard time squeezing between the MK64FX512VDM12 ic. The VLQ12 are way out before the become available.
    I will do the board with .15mm just the be safe if it gets rejected.
    1st time with this IC.

  4. #4
    Senior Member PaulStoffregen's Avatar
    Join Date
    Nov 2012
    Posts
    20,306
    The traces on the Teensy 3.5 & 3.6 PCB are 5 mils (0.127 mm) wide in the BGA area, and 7 mils (0.178 mm) on the rest of the board. Most of the traces on the bottom layer are 8 mils (0.203 mm). Most power is routed as planes on layers 2 and 5, but a few power traces on the internal layers are 10 to 15 mils wide.

    The vias inside the BGA area are 19.2 mils (0.488 mm) diameter, and the vias on the rest of the board are 25 mils diameter. The BGA pads are 0.5 mm diameter. The vias have a staggered offset relative to the BGA pads, only 34.3 mil (0.874 mm) apart between even numbered rows and 44.4 mil (1.128 mm) apart between odd numbered rows. This staggered arrangements allows 50% more horizontal routing. One horizontal trace can still pass between the 34.3 mil spaced vias on the internal layers, but on every other BGA row, two traces can pass between the 44.4 mil spaced vias. You probably would not need this trick for a normal PCB design where traces can escape from the BGA in all 4 directions, but it's pretty much essential to achieving the escape routing on the limited area of the Teensy 3.5 & 3.6 layout.

    While I used 0.5 mm diameter pads, apparently going down to at little as 0.4 mm is acceptable. But smaller geometry pads do require different manufacturing steps to build the boards.
    Last edited by PaulStoffregen; 02-22-2018 at 07:15 PM.

  5. #5
    Senior Member
    Join Date
    Oct 2014
    Posts
    167
    Thanks Paul, this will help a bunch

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •