FEDEVEL
Platform forum

Didan , 01-18-2019, 10:41 AM

Hello everyone, I followed all steps from videos and I finished board - Sch + Layout, however Im facing troubleshoot here because after i've done Power plane and high speed signal plane, GND connections seems unconnected and IDK why. I drew a polygon om BOTTOM for GND and I reduced problems with unrounted and net antenna but on original layout theres any gnd plane on BOT, its only necessary place gnd vias and polygons to ensure strong gnd connections between importants components which need it as talked on videos. Someone can help me to solve it ? I dont wanna draw gnd plane polygon for it, just using gnd vias as original layout. Whats wrong on my layout? Should be schematic ? I compared my project with Robert and its the same now, all polygons, location x/y for components and whole rest to make sure i will do everything right but I just need solve it to make output job files and send for production...

robertferanec , 01-21-2019, 06:48 AM

You need to assign GND net to the planes on L2 and L5. This will help you https://www.fedevel.com/academy/updates/ especially this: https://www.fedevel.com/welldoneblog...e-new-old-way/

Didan , 01-21-2019, 07:09 AM

Hi @robertferanec, thanks for answer. Well, I assigned plane P1 and P2 to GND but looks same, unconnected GND and whats weird when I look on your board demo, theres any assigned net for plane. why?

robertferanec , 01-21-2019, 08:32 AM

You have different thermal relief set - use direct connection. That can cause the problem (some VIAs may be disconnected as copper cant flow to them). Go to Design -> Rules -> Design Rules -> Plane -> Power Plane Connect Style -> PlaneConnect and change it to direct connect:

Didan , 01-21-2019, 08:44 AM

Oh @robertferanec you got it. I remember that step on video I thought Ive done it, but maybe I forgot, you explained it. Now I think project is well done and I can generate gerbers and finish course. Thanks for this course I learned so much, i think was almost 20h dedicated for practice on this course. Do you suggest where I can send gerbers file to manufacture board? Where did you send yours? Can you teach one thing please, about quotation I have some doubts about what are differences and best option to manufacture this board. For instance, I was quote on pcbway, which should be the best configuration for this board switching power supply you taught on course? I marked with red topics I wanna understand better.

robertferanec , 01-23-2019, 08:21 AM

The last time I used for this PCB https://jlcpcb.com/ ... it costed 212 (including DHL delivery)

Didan , 01-23-2019, 10:03 AM

Dear @robertferanec Do you have any link or video explaining how to set up manufacture settings on website like jlpcb? Im looking it and about impedance, for instance, Do I need to worry about it? About surface finish do you have any video explaining differences about it? Back to impedance, if yes they have a page to calculate it and how should I set it correctly? Well, many questions and as possible i google it but as you created course nad had manufactured switching power supply board your feedback is very welcome Thanks

robertferanec , 01-25-2019, 02:21 AM

I have never used cheap PCB manufacturer for impedance controlled PCB. I am not sure how much to trust the result. If you are not sure, for standard digital signals you can use 50OHM, but I usually go for cheapest PCB and a little bit wider track (e.g. 0.2mm - 0.3mm track width) .. again this is only for simple PCBs where impedance is not important and I just need cheap PCB.

Surface finish - I normally use Gold (ENIG for standard PCBs), but for home prototypes and cheap PCBs I go for cheapest (HASL with lead). Just be aware, PCBs in EU products need to be lead free - so you can not use HASL with lead for products). HASL = like tin

Some settings just do based on your PCB - minimum track/clearence, minimum hole (remember what is cheapest and use it next time in your PCB - you can save a lot of money this way). I tent VIAs (means they will be covered with the green color). Standard PCB thickness is 1.6mm. Finished copper - 1oz is good for standard PCB (that is what I normally use, for signal layers I also use thinner layers e.g. 1/2 oz .. but it is only to get right impedance which is not case in cheap PCBs ... so 1oz is ok). If you would need to design PCB for higher currents, go for more oz.