Antichambre

dipCoreF4 and dipBoardF4, a compact Core.

96 posts in this topic

I am sourceing cheap alternatives to mouser, for my projects, and for you dipcorei want to try https://lcsc.com for some of the parts. (some parts i already put in your dipcore wiki boom)

 

some questions:

RESISTOR:

do they need to be 1/4W or are there some where 1/10W is enough?

 

CRYSTAL:

i dont know what Quarz you take... but when look at the footprint then it looks like it can only be "Reflowed" ? since the solder points are under the crystal? most of the Crystals i found have it under the Body...

for example: 8MHZ 12pf

how we solder them?

C12-C13:20pf - had to be changed when using a other crystal.... so for the example above i would replace it with 12pf (or is there more i  have to think of?)

Edited by Phatline

Share this post


Link to post
Share on other sites
27 minutes ago, Phatline said:

i want to try https://lcsc.com for some of the parts.

a quest the Resistors, do the need to be 1/4W or are there some where 1/10W is enough?

It depends which one, better to keep 250mW for low value resistors (<100?). This can be optimized later.

Share this post


Link to post
Share on other sites
54 minutes ago, Phatline said:

CRYSTAL:

i dont know what Quarz you take... but when look at the footprint then it looks like it can only be "Reflowed" ? since the solder points are under the crystal? most of the Crystals i found have it under the Body...

for example: 8MHZ 12pf

how we solder them?

 

On 07/10/2018 at 6:14 PM, Antichambre said:

Note to the beta testers:

  • The 8MHz Quartz is not easy to find in this package(proprietary one), but I ordered some and I will put enough for you in the envelope.


Hot Air station is recommended for this one. It will be corrected in next version.

Don't change load capacitor, it's fine. https://blog.adafruit.com/2012/01/24/choosing-the-right-crystal-and-caps-for-your-design/

Best

Bruno

 

Share this post


Link to post
Share on other sites
1 hour ago, Phatline said:

some parts i already put in your dipcore wiki boom, under "others"

Thank you.

Share this post


Link to post
Share on other sites

Sorry guys!!! There will be some delay :(


Fichier%2015-10-2018%2023%2001%2032.jpeg

Fab made an error, I've found a workaround for this one as I can check everything but the other boards are just good for trash.
Fichier%2015-10-2018%2023%2045%2000.jpeg

They connected VBUS to Ground internally, via and pad are connected to the wrong internal plane I think. Fortunately VBUS and 5V are separated by a fuse, there's no more protection but I can switch it On

Fichier%2016-10-2018%2000%2035%2057.jpeg
 

And check everything before they fab it again.

 

Edited by Antichambre

Share this post


Link to post
Share on other sites

Sorry to hear Bruno. Where did you get your boards made?

Share this post


Link to post
Share on other sites

Osh-Park but it's the first time, their first mistake and we are far from first order... communication is good, they answered me in the hour. Dan already refund me some as a gift just for the time spent on soldering and wasted components.
Now they are looking for the reason of the error, they are checking their production line. They need to understand before fab it again. This is fine for me, I've got one working I can check everything and maybe leave beta version on next fab directly.

I suppose it can happen to the best too. Nobody's perfect.


 

Share this post


Link to post
Share on other sites

Then finally, I've got 3 issue.
- Because of a plated Slot VBUS is connected to GROUND on the dipCoreF4.
- Because of a plated slot DC-IN is connected to GROUND on the External power module.
- From the same brand and range I put a RJ45(8p6c) connector model instead of a RJ11(6p6c) on the MCAN Module.

But I found a workaround for first and second issue. For last, MCAN module doesn't matter for the moment...

So I decide to not refab it, they are working, enough for our tests, I prefer to keep the money refund for another and double checked run or something else.

I will change fab too for next run. They sent me a dipBoard with copper totally scratched and cut under soldermask then there was no visual check, no quality control. That's definitively not good :angry:

Beta testers, I will send you the boards on Monday... Hope you will understand, I will provide you some thin cable and heat shrink tubing I used for dipCoreF4 workaround.
Next run will be perfect and ready to run your application cleanly.

I'm currently finishing the MIOS32 modification for this Core, I will share pictures and example in the next days.

Best
Bruno


 

Share this post


Link to post
Share on other sites

You use EAGLE, correct? One thing I remember is that slots are always a "hack" without proper DRC. You have to manually place keepouts/restricts on internal layers.

Also note that some fabs will not like overlapping drill hits ("combo holes"); for them it's a risk that their drill or milling bit slips on an edge and breaks.

Share this post


Link to post
Share on other sites

This is exactly what happens, pad shape on internal layer are not extended like bottom and top are, then larger plated slot merged GND and VBUS on internal layer.
The only way to avoid it and keep the slot is to add copper with the extended pad shape like this:
slot%20correction.png?raw=1
Now I know it!!!
 

Share this post


Link to post
Share on other sites
35 minutes ago, latigid on said:

Also note that some fabs will not like overlapping drill hits ("combo holes"); for them it's a risk that their drill or milling bit slips on an edge and breaks.

Yes I know but I took that risk, cause I already did it by the past and it was working. But to avoid any risk I will make slot for each "combo holes" on next run...

Share this post


Link to post
Share on other sites

Yep, BLM 16x16+X and 'ELO. No problems, just don't forget to set isolate to a reasonable value!

Share this post


Link to post
Share on other sites

What "isolate" means? Clearance? And what is reasonable?
I use 5mil clearance for dipcoreF4.

Share this post


Link to post
Share on other sites

Isolate is a polygon parameter that automatically keeps distance to routed traces, drill holes and pads. I am very conservative with isolate (0.5mm/~20mil).

Clearance is the distance between two routed traces, also related is the distance between copper and a dimension (edge of board or slot).

Conservatism is overkill, but the more conservative, the less chance of something going wrong. E.g. imagine a piece of dirt or dust on the photomask. If the clearance is too low, the fault might manifest into the production and short or cut a trace. Just because the fab gives low min clearance rules, doesn't mean they're a target. 

Just my opinion of course, please decide what's right for you.

Share this post


Link to post
Share on other sites

Yes for sure. But I hope our fab works in white room ;)
dipCoreF4 is a tiny board, 20mil is just impossible in that case.
I know Eurocircuit will do it perfect, they are expensive but the board size is small. Price is good enough from 25 pieces.
I will check that later and PCBA too...
Thanks Andy
 

Share this post


Link to post
Share on other sites

Absolutely! 

I think Eurocircuits boards will be dependable right down to their minimum design rules.

Share this post


Link to post
Share on other sites

Eurocircuit made the OLRE16(green version) which was absolutely perfect, very precise, the most beautiful board I even made.
I try to work with them, but they are too much expensive for Prototype quantity, then I used OP for that part. Grrr
And I'd got a lot of problems with Seeed production with the exactly same design same rules of the OLRE16(black version on pictures).

Share this post


Link to post
Share on other sites

Im with Andy, I always make the isolation as BIG as practical.  If you have to pack it in, you have to pack it in but only do so where absolutely needed.  You can pour different polygons with different isolation on the same net too if you need it tight one place and not another.  Every time i've gotten bad boards from OSHpark (3 times this has happened) it was because there was a super tight/dense space and the etching didnt get all the copper.  They are probably way more sensitive to this than other fabs since they do big ass boards with many designs and i bet its easy to have issues etching something that size.  

I think it boils down to getting a handle of what the fab says they can do and what they can actually do reliably.  I had problems with Seeed with my first order there and never went back, the etching was rough, the soldermask was poorly registered, just blah everywhere.  JLC i'll use for big stuff since their pricing is good but small stuff they have issues with clean screens even at their minimum text size spec.  PCBway has nice machines but they take a maximum X size of 110ish mm so big stuff gets pricey there too,  They cant do small text like OSHpark can on that machine.  So it's a mixed bag always where ever you go.  I go through a thousand boards a year and have yet to see a etching fault on any of the Chinese fabs which is why I dont use OSHpark anymore, it was a convenient service 5 years ago but the prototype biz in china has exploded and you can do much better for much less time and money.  Standard turn around for protos is 2 days at any place out there

Edited by Altitude

Share this post


Link to post
Share on other sites

For me, THEY provide a DRC we have to follow then they HAVE to respect it too. Or they can not provide the service.
But I never got any isolation issue with OP, and this is not the problem this time too, unfortunately.
Except plated slot error, everything else seems fine for the moment included USB which has sensitive traces.

First I was disappointed but I quickly found a workaround and they are usable for dev, that's fine. :)
 

Share this post


Link to post
Share on other sites

and thats why we run prototypes :) 

 

 

IMG_20181020_070248.jpg

Edited by Altitude

Share this post


Link to post
Share on other sites

Even with all the red stripes this is beautiful, there's a lot of work in this, what it is?

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!


Register a new account

Sign in

Already have an account? Sign in here.


Sign In Now