Forum - EasyEDA - An Easier Electronic Circuit Design Experience

Latest Topics Latest Replies EasyEDA Std EasyEDA Pro JLCPCB LCSC OSHWLAB General Discuss

PCB SMT 3D/CNC Feature Requests Bug Reports

BGA JLCPCB pitch 0.5 mm.

3571 10

Remy 1 year ago

Hi, I am designing a board with a eMMC (from the JLCPCB parts list ([https://jlcpcb.com/partdetail/Samsung-KLMAG1JETDB041/C499919](https://jlcpcb.com/partdetail/Samsung-KLMAG1JETDB041/C499919)) and it has (like the others) a 0.5mm/19.7mills pitch. Therefore I need a clearance of 0.082mm/3.2 mils and a 0.082mm/3.2 mils trace to fanout. I contacted the support, but the response is not very clear. I also doubt if the lady understands me. The min. Pad is 0.25mm/9.85mils, so that gives me 0.25mm/9.8 mils of space between the pads. The proposed clearance is 0.089mm/3.5 mils and min trace 0.089mm/3.5 mils. That makes 3x3.5= 10.5 mils (0.267mm). Anybody experience with them? ![Screenshot 2022-10-01 130859.png](//image.easyeda.com/pullimage/eGqZABR1cnWdLJddm6pxe1i3DdBHpsI34q88kVZ1.png) ![Screenshot 2022-10-01 130842.png](//image.easyeda.com/pullimage/fmYLahNYfeixZ9MmTbrUTWIToFzatTWLtajaMuVW.png) ![Screenshot 2022-10-01 130814.png](//image.easyeda.com/pullimage/LjrpT1537cbX1TNhF0l37zA5zUFdgnhb9PjQb2rb.png) ![Screenshot 2022-10-01 131106.png](//image.easyeda.com/pullimage/pqfI6HGo5pBtlDNvlKxu5vHHOhsHGk5prLstLY2c.png)

Safari 16.0 iOS 16_0

Comments

andyfierman 1 year ago

Bearing in mind that english may not be the first language of JLCPCBsupport and that you are swapping between mm and mils with no clear description, calculations or diagrams to illustrate your question, it is quite likely that there is some confusion or ambiguity in the response to your enquiry from JLCPCB. A clearly and consistently dimensioned diagram would go a long way to help answer your questions.

Chrome 104.0.0.0 AndroidOS 10

andyfierman 1 year ago

Does this topic help? [https://easyeda.com/forum/topic/5mm-BGA-PCB-design-61c7fe69e3b742acb725d86adeb2f5c8](https://easyeda.com/forum/topic/5mm-BGA-PCB-design-61c7fe69e3b742acb725d86adeb2f5c8)

Chrome 104.0.0.0 AndroidOS 10

Remy 1 year ago

@andyfierman Hi Andy thx for your reply. My post is not meant as to be mean to JLCPCB or the employee, I just want to have some clarity. I added some pictures to make it more clear. Because the minimum pad size is 0.25 mm (9.85 mils) and the pitch is 2x0.25mm = 0.5 mm, I only have 0.25mm/9.85 mils between the pads to put the traces. By the way, I use Altium Designer. In that 0.25mm/9,82mills space I have to consider: * clearance between trace and pad, minimum 3.5mils/0.089mm. This has to be counted twice, because of pad - trace - pad. * minimum trace width is 3.5 mils/0.089mm. So, twice the clearance and once the trace accounts for 3x3.5mils = 10.5 mils or 0.267mm. To be clear: the part is offered by JLCPCB itself, for assembly. Of course I can order others myself, but the purpose is to let them assemble the boards. So maybe better asked, how absolute are those minimums. Maybe anybody has experience with a local change in rules (only for this BGA) and use 3.2mils/0.082mm as clearance ánd min. trace width.

Chrome 105.0.0.0 Windows 10

Remy 1 year ago

NB: the last picture is from Texas Instruments: [Link](https://www.ti.com/lit/an/sprabb3/sprabb3.pdf?ts=1664533762736&ref_url=https%253A%252F%252Fwww.google.com%252F), page 12, to make it more clear.

Chrome 105.0.0.0 Windows 10

JLCPCBsupport 1 year ago

@remy_5896 Hello Remy and thank you for your post. I wonder if you have tried to add some Vias to rout the inner Balls! Considering your routing requirments (Clearance) this is not possible to go for under 0.09mm trace width which is our JLCPCB smallest trace width that could be acheived only for 4-6 Layers PCB design.

Chrome 106.0.0.0 Windows 10

Remy 1 year ago

Hi, thx for the reply. The thing is, I have to access the red pads and can’t cross between the pads. So the green pads I could access, not the reds. But maybe I make a failed judgement, not very familiar with BGA’s. ![509FB50A-23BD-4AFC-BD26-3622FD7B36E9.jpeg](//image.easyeda.com/pullimage/UOpT3jFWlDKvAXQPyFljkH59yCCpYnWP0uz57v7y.jpeg)

Safari 16.0 iOS 16_0

JLCPCBsupport 1 year ago

@remy_5896 If these pad around the red ones are not connected (NC Pads) like A1 A2 A3 A4 etc then maybe you cross them to reach the red pads, seems like a bad idea but maybe it could help as long as these blank pad are not connected.

Chrome 106.0.0.0 Windows 10

Remy 1 year ago

In the end I just uploaded my project with clearance/trace smaller than officially supported by JLCPCB and the endresult is that it just works! ![Screenshot 2022-10-31 100516.png](//image.easyeda.com/pullimage/nHttQz2VeTgFmpZKlgUKRzYdRLFT2AkMCXC4gMVn.png) ![Screenshot 2022-10-31 100415.png](//image.easyeda.com/pullimage/DF8NJzrKVEFx1HljH88X7yGh8FtuqdMSb8UMkk7a.png)

Chrome 106.0.0.0 Windows 10

andyfierman 1 year ago

@remy_5896, What dimensions did you use?

Chrome 104.0.0.0 AndroidOS 10

Remy 1 year ago

Hi Andy, because of the 0,50mm pitch and 0,25mm pad size, there was only 0,25mm free space for twice a pad-trace clearance and a trace. I used a 3.2 mils trace clearance and 3.2mils trace width.

Chrome 106.0.0.0 Windows 10

你现在访问的是EasyEDA海外版，使用建立访问速度更快的国内版 https://lceda.cn(需要重新注册)
如果需要转移工程请在个人中心 - 工程 - 工程高级设置 - 下载工程，下载后在https://lceda.cn/editor 打开保存即可。
有问题联系QQ 3001956291 不再提醒

Cookie Notice

Our website uses essential cookies to help us ensure that it is working as expected, and uses optional analytics cookies to offer you a better browsing experience. To find out more, read our Cookie Notice

Unleash creativity, start design now.

Cookie Notice