Announcement

Collapse
No announcement yet.

castellated mounting holes

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

  • robertferanec
    replied
    I agree with beamray. Ask your PCB manufacturer for recommended castellated hole dimensions. I have not had any problems with that before (I just mentioned, these are castellated holes and they just did it).

    For example, this is from jlcpcb:
    https://jlcpcb.com/quote/pcbOrderFaq...llated%20holes

    How to make castellated holes in your design?
    Please make sure a via or plated hole is added directly on the outline of the boards where the plated half hole is required.
    Ensure that half of the via is on the board and half is on the outside of the outline.

    BTW the following rules should be followed:
    - Copper layers (GTL and GBL): Copper pads on both top and bottom copper layers for each castellated hole.
    - Solder mask layers (GTS and GBS): Solder mask openings on both sides.
    - Drill layer (TXT/DRL): A drill hole for each castellated hole.
    - Mechanical/Outline layer (GML/GKO): The outline should cross the drill hole.

    Notes:
    1, When "Yes" option is checked on the order form, we will make the half holes found in your design to be plated with copper, it will cost you extra fee for half holes.
    2, If "No" is checked, the half holes will not be plated with copper.
    3, To make Castellated holes, the hole size and space need to be 0.6 mm at least.

    Leave a comment:


  • beamray
    replied
    Not more than 2 month ago I have done number of RF modules like that:
    I Used usual through hole pad with offset of pad to hole centre. I was okay. I always make sure that in fab notes layer I had noted that THOSE are castellated.
    Keep in mind solder temperature for both modules ( you can not use same solder) and make sure that PCB is not more than 0,75% twisted (but not more than 0,3mm). Also make sure that castellated holes are spread through perimeter of the board. And consult your manufacturer for castellated hole minimum diameter and centre to centre and edge to edge distances. I use 0.8,, diameter and about 2 mm centre to centre as minimum.

    Leave a comment:


  • NormsBreaker
    replied
    Click image for larger version

Name:	images (1).jpeg
Views:	343
Size:	21.2 KB
ID:	14536 Hey robertferanec!
    First of all, I would like to thank you for your lucid videos. They're awesome.
    Coming to the point, I am using through-hole pads and vias to achieve castellation. But I'm having trouble cutting them down in half. Can you please help me out with that? It isn't given above.
    I am trying to achieve something like that on my board.
    Thanks in advance!
    Last edited by NormsBreaker; 06-01-2020, 06:19 AM.

    Leave a comment:


  • IvesPhillips
    replied
    As per my experience with the castellated holes you must use the through hole pads and cut them in half. Hope it ll work for you. Also if you are looking for more precision then you can also go for the SMT pads and the placed VIAs with them. You can make the row of pads and add them at the edge of PCB.

    pcb manufacturing
    Last edited by IvesPhillips; 11-06-2015, 01:41 PM.

    Leave a comment:


  • robertferanec
    replied
    Hi mortiz29772, thank you I am very happy you like the videos

    About castellated holes. I used it only once - as suggested by others, I simply just used through hole pads and cut them in half - worked oki (to be precise, I used SMT pads and placed VIAs into them ). See the attached pictures.



    Click image for larger version

Name:	castellated holes - bottom.png
Views:	1393
Size:	200.6 KB
ID:	269


    Click image for larger version

Name:	castellated holes - 3D view.png
Views:	1532
Size:	375.8 KB
ID:	270

    Leave a comment:


  • mortiz29772
    started a topic castellated mounting holes

    castellated mounting holes

    Hi Robert

    Have you figured how to make castellated mounting holes at the edges of the pcb, in order to make a pcb that would be mounted on top of other pcb? I haven't; most of the forums suggest to make a row of pads and put them at the edge of the pcb, but I was wondering if this feature has been already implemented on Altium; I can't imagine they have implemented flex pcb's and no castellated holes. Any advice would be highly appreciate. BTW your videos are really helpful; you rock!!! Greetings.

    Manuel Ortiz
Working...
X