JLCPCB: Need clarification about JLCPCB Capabilities
413 14
iot-hub 2 months ago
Hi guys, I'm making pcb design with DR-QFN package and plan to make order for JLCPCB. Checked capabilities [here](https://jlcpcb.com/capabilities/Capabilities) and one think not clear for me. Please clarify if you known and can help. DR-QFN have two lines of pads: outer and inner.Clearance between outer pads = 8 mil or 0,20 mm. From requirements it's ok: ![img0.jpg](//image.easyeda.com/pullimage/TXMUjRd1xdQyAYJ9jcntEwFFTBc56mqWEbGySAow.jpeg) But for inner pads I must to create track only between two outer pads. Like in the picture: ![img1.jpg](//image.easyeda.com/pullimage/B4immriSloK54cgK7IKJJNLLgkJ8m3mWDkTvjlyA.jpeg) According JLCPCB Capabilities I see what Minimum allowed trace width and spacing will be 5mil (0.127mm) for 2 layers or 3.5 mil for 4+ layers in 1oz pcb. In my case it's requre 5 (spacing)+5(track)+5(spacing) = 15 mil or 0,38 mm between pins 48 and 50 what twise greater what I have for fabrication. Reference: ![img2.jpg](//image.easyeda.com/pullimage/Ul409UtcykQ5IAZWZYaWFWXzEiNMDkn0IArmBD5Q.jpeg) In this case looks like this chip and my requirements out of capabilities of JLCPCB. BUT(!): If I scroll down to BGA requirements I see min distance between balls = 5 mil or 0.127mm but what equals to minimal trace requirement abowe for 1-2 layers on only to 1,5 mil less what allowed to 4+ layers boards as I understood JLCPCB not expect what all balls will be floating without traces to some other pads because they not allowed by requirements. ![img3.jpg](//image.easyeda.com/pullimage/SMCkavAhnkmet2CQyDGmMjZpmcqEwqchewe9oSiJ.jpeg) How to understand this? Is requirement for spacing works only for traces but not working between trace and pad or ball? What is minimal spacing between pad and trace will be in this case? In my case I can forgot about spacing bettwen trace and pins or can forgot about order from JLCPCB?
Comments
JLCPCBsupport 2 months ago
Hello ; Thank you for posting your question here. Please make sure that the clearance (outer pad to pad) related to you components is really 0.2mm. If you provide the component reference, we can better assist you. In many DR-QFN parts the outer pads clearance is 0.45mm Your request is totally clear and very well explained, please provide us with the requested information to help you more in this. Thank you.
Reply
iot-hub 2 months ago
Hi JLCPCBsupport, my component is MT7688AN. You can found datasheet [here](https://s3-ap-southeast-1.amazonaws.com/mediatek-labs-imgs/downloads/1f9d1b96f0f20242df0e3826fccc9da0.pdf?response-content-disposition=inline%3B%20filename%3DMT7688_Datasheet_v1_4.pdf&X-Amz-Content-Sha256=UNSIGNED-PAYLOAD&X-Amz-Security-Token=IQoJb3JpZ2luX2VjEDUaDmFwLXNvdXRoZWFzdC0xIkcwRQIhAOADK2ZdeRxT1nXb2u3pBzWKtzYMov4lm9%2BDHzurpw1cAiAdxqj8Mv2K5f1C%2BZyaVqcpj7us%2BTCL4Xhw18g6DEzdxyq%2BAwg%2BEAEaDDQ0OTY5Njk5MjA2NiIMkGQp1pMWcMPhS%2BpMKpsD1vBwHzPjRcGqute7kxC57j4YCMSssyGDMWZDb10K5xhxIaA78FRYvUJ%2FcYVAgX5PXXUGK1HJ6YbPScg5kV0lkkSu4D5Vez6Vk2JzVEFyMiqO9eb5PscRQrciJzQ5tctNQzAG83ged6Ndns0fZrlEC4AO0MVC%2BwqM5JaLexUQao6W4uJFeOolS2GVmmC5PBMv5IqfrjW4xBCL97mGzzZev3Qb9C%2Fe%2BA6I3SZZZH11K1mMWFHysgZVbWFofqcD%2BwxhR0He68dbH0P%2F%2FeD8GAKISV0Xncie6clrfBKlAGQYVJXiNq0SNVNVGqsBQgSJy0JpAQTYoHzMAPP8kJnHVQ3NoihUmDdA21X74aGTRG8%2FeaoQgoWApGA%2FIrjjL727k3h%2FPp9HK7eeDSsDsZJrHs%2FGXaUJEPon8vFGlG%2FsP5SlZ1C8pHtLUXbj4agOEGdpH3zr%2BWpbaMJgvRrjIPlQExM81CDuzwp8rFrlRZMsvrW1kRiEYhsgjP3t6RZFklLHfiubSZGLz0LnDlagOnsp3pvFk7cf7Mbj3%2FnCTf31MNfF4foFOusBXvPlVpS6lHMljSGiEHNTZQvQ58ElyxympdSzbl915j6cR9av%2BxWUDEu2UvT%2FF%2F0MHzv6wbfB9tGzqZAz05HOSTBfai%2B%2BZL3K22eggKLI%2BmcyHSdTvvxb8vUAA7UwmQP%2BOgosKaO3%2FisQvdQB8mEQz%2BZwo5owqnEeyVxXj%2FBrCLeNvIroFD1TaCzJkIF8K2ybkHs9wGVYslVHEocJurXhbobPJxeyBIZP2%2B%2Ft8hcHggExCnS2ju87PNINwju%2FBnogzzZ8iPrLvQsYqasl6jvlYF5RMNEMaoDBE8zASEfQwSalyuMNoTADCBzTKg%3D%3D&X-Amz-Algorithm=AWS4-HMAC-SHA256&X-Amz-Credential=ASIAWRNAHRNBNLAO2BVY%2F20200909%2Fap-southeast-1%2Fs3%2Faws4_request&X-Amz-Date=20200909T055740Z&X-Amz-SignedHeaders=host&X-Amz-Expires=600&X-Amz-Signature=1038f0f93c55e27c9ecee8daff71e08dd12f60e1ff7331431a7cfafe6c5857fe). Package Physical Dimensions desicribed in page 43 in section "4.9.2 DR-QFN (12 mm x 12 mm) 156 pins". Few screenschots to minimize your time: ![img4.jpg](//image.easyeda.com/pullimage/LKji7EQMz49EvzaIvUbRWJmElcGb6wtSoM8ZCSxs.jpeg) ![img5.jpg](//image.easyeda.com/pullimage/7pwq3MuP92ddSC8v9SpZ5zYfzKWW97gPxXCCk7fn.jpeg)
Reply
JLCPCBsupport 2 months ago
@iot-hub Hello ; Thank you for the useful information. Regarding the datasheet that you have provided, the pad to pad clearance of the outer line is 0.2mm if we consider the maximum lead width, so if we measure it as follows : The measure of lead pitch (eT) = 0.5mm related to the **B**asic **S**pacing between **C**enters The lead width max (b) =  0.3mm Then the clearance outer line pad to pad is eT - b = 0.2mm For JLCPCB capabilities the clearance trace to pad is 0.127mm and minimum trace width is 0.127mm so in order to route similar component you need a sum of : 0.127 mm + 0.127 mm + 0.127 mm = 0.381mm at least which is not possible in your case. We are sorry that we can't produce this part for you regarding our capabilities. Thank you again for the time taken to write your post here.
Reply
ResistanceRoom 2 months ago
You don't need to trace between the outer pads to connect to the inner ones. You can use any other layer (bottom one if it is a two layer board) and then put a via under the body of the component. Like so: ![image.png](//image.easyeda.com/pullimage/9QhfSqkFRbo4HbBKUdrUoc2fHWE4Gne2YvhCvTtF.png)
Reply
JLCPCBsupport 2 months ago
@iot-hub @ResistanceRoom This could be a solution only if you find a way to route all the inner 76 pads. The part is really tight and it has 19 pads in each of it inner lines which is a total of 76 pads to be routed in a surface of 12 mm x 12 mm. Please to consider the minimum Via diameter which is 0.6mm for single&double layers PCB and the minimum clearance Via to Via which is 0.254mm. so if we make a two lines of Vias for each of the inner lines there will be a sum of 0.6 mm x 10 Vias = 6 mm + 0.254 mm x 9 spacing = 2.286 mm the total space needed is 6 mm + 2.286 mm = 8.286 mm Then if we consider two lines of Vias then we need to take a Via to Via clearance of 0.254 mm Please find more explanation in the below image : ![route-1.png](//image.easyeda.com/pullimage/nR0wXJkJgsnVAuiPfpW3gq84pqkACW8i8Wf9t73G.png)
Reply
iot-hub 2 months ago
@ResistanceRoom, @JLCPCBsupport, thanks for you proposal. It's first what I start to did but not finish and asked a question. As I understood - this option is work if in chipset I have possiblility to connect some inner/outer pads like 1 inner ground pin and 1 outer ground pin nearby for example. Need to check this. @JLCPCBsupport, BTW: Returning to BGA requirements. In JLCPCB allowed space between balls - 0,127mm. Minimal trace or clearance are equals the same 0,127mm too. How to trace inner balls in this case or maybe it's some missprint in requirements?
Reply
iot-hub 2 months ago
Have this: ![img6.jpg](//image.easyeda.com/pullimage/ezk8LF2h1vnaunPYecJ5h8qoyTtyBYeXdtVm0C05.jpeg) via size 0.45/0.25 (4+ layer board requirements) but based on last comment from @JLCPCBsupport looks like not possible to meet to "via to via" requirement, right?
Reply
iot-hub 2 months ago
Update from my side. Please see picture below. Looks like I have possibility to make PCB. Legend: Grid size: 10 mil (0.254 mm) ![image10.jpg](//image.easyeda.com/pullimage/9gdbd4nciovaqv5yM4KOSE0sb2EHPAFhWQjAbRGx.jpeg) Pad to Pad clearance(Pad with hole, Different nets): 21.25 mil (0.54mm) - looks OK. Pad to Track - 7.87 mil (0,2mm) - looks OK. What is missed? Thanks.
Reply
JLCPCBsupport 2 months ago
@iot-hub Hi again Good to see the update which looks positive as a result. You wrote : > Pad to Pad clearance(Pad with hole, Different nets): 21.25 mil (0.54mm) - looks OK. You don't have any Pad with hole in your image, so please check, you better use the Pad to Pad clearance | | | | | --- | --- | --- | | Pad to Pad clearance(Pad without hole, Different nets) | 0.127mm | ![](https://jlcpcb.com/client/image/pcbCapabilities/PadClearance.22a09e99.jpg) | About the BGA, that is not different but what we have mentioned is the minimum spacing between balls and if you get a component that reach this clearance than routing it will be through Vias the way you did with your DR-QFN package part and it will be almost something like the following image : ![505661579542024505.png](//image.easyeda.com/pullimage/0HtAj3dR1S8fNteyddnSZww8Rp0B2t1dyZaeDWQI.png) Have you done finished the DR-QFN part? Do you still need any support? Thank you again for your post.
Reply
iot-hub 2 months ago
HI @JLCPCBsupport, thank you for you response. \>\> Have you done finished the DR\-QFN part? Do you still need any support? Give me one day plz... I'm in the finish stage. What is better to check: share some screenshots with info or maybe share project to check/validate?
Reply
JLCPCBsupport 2 months ago
@iot-hub Hello ; You can share the project Ok
Reply
iot-hub 2 months ago
Hi @JLCPCBsupport, I copied project and removed all unnecessary part except DR-QFN + one part for text connection. Project available [here](http://www.easyeda.com/iot-hub/dummy-test). Checked in JLCPCB design rules. Looks ok from DRC errors perceptive... but :) ![image11.jpg](//image.easyeda.com/pullimage/AuI1gIO3UmSJ1PUBg6Byy52dSqqUvM7KcVxADETL.jpeg)
Reply
JLCPCBsupport 2 months ago
@iot-hub Hello ; Regarding the method, you are in a good road ![Capture.JPG](//image.easyeda.com/pullimage/uf4Ru2jA4c6Gtp4pSaDj92nXAeEmZk3kGnsfjPw9.jpeg)
Reply
iot-hub 2 months ago
Hi @JLCPCBsupport, I'm really approciated for you help. Thank you very much!
Reply
Login or Register to add a comment
goToTop
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
svg-battery svg-battery-wifi svg-books svg-more svg-paste svg-pencil svg-plant svg-ruler svg-share svg-user svg-logo-cn svg-double-arrow
We use cookies to offer you a better experience. Detailed information on the use of cookies on this website is provided in our Privacy Policy. By using this site, you consent to the use of our cookies.