Single-Board Universal Module

I'm using the 4 layer rules from here: support.oshpark.com/support/articles/400...10-eagle-design-rule which seem to agree with the 5 mil trace and space and 4mil annular ting rules on their specs page. I get 140 errors, with about ~1/3 of them clearance. Make sure the layers are visible, or they don't show up in the DRC list. A whole bunch of the other DRC errors are just library issues and can be approved. I don't really think this is the cause of the power to ground short though. They're all clearance between a via and a pad of the same signal.


I see lots of people remove too much solder from surface mount pads with solder wick while cleaning up bridges. It's also really easy to overheat and lift pads while using it. There are some hollow shaped chisel tips for the Hakko iron I have that are great for removing excess solder and cleaning up bridges. They have a little bowl in the flats of the chisel, which holds on to the solder. I'm not sure what iron you have, but it might be worth looking for something similar for your iron.

Yeah, I have the 0.9 layout. I wonder if maybe we have different restring values, causing the annular ring on the vias to be larger for me. If you have no DRC errors, I'm sure the problem is on my end.

Found it.. The DRC rules used on the layout in the repository have 0 mil minimum for same signal clearance. Not a huge issue, but that explains why we were getting different DRC results.

PhracturedBlue, what microscope do you use? How does it compare with glasses?

Well, another week and no boards for me. Hopefully they show up next week.

Nice project!
I just did a pull from bitbucket.org/SadSack/universaltx-4-layer/downloads and looked at the schematic. (june 3, 2014)

The DRU still comes up as a 2-layer board?
EDIT: I just pulled V0.9 which has 4 layers. This is not the typical stack-up which has ~9mil dielectric on outer layers.
9 mil dielectric is doable for FR4 keeping 50 ohm lines at sane widths.
(strip-line should be 14 mil wide on 8 mil FR4 ~ e=4.4)
The 1.5 mm dielectric would make those 9 mil lines 133 Ohm.


This would be a typical mass production type board, 1oz. outer, 1/2oz. inner copper and ~ 8 mil dielectric.




Just quickly breezing tru schematic for possible trouble, and I saw one that bit me once;
The SKY13384-350LF U6 pin 15 input as well as the RFX2401C U5 pin4 are both have DC, and there is no DC-blocking cap on this line. Odds are the DC-levels are not the same. The other ports on the 4-way switch have DC-blocking via the matching caps, which should suffice. The RFX2401C has DC on antenna, and to reduce chances for mishaps a cap here would not hurt.

The SMT USB connectors are not as robust as the thru hole type, H2960TR-ND. The strength of copper adhesion to the FR4 is not that impressive.

Did you consider a SAW filter on the PA input? You get a 2dB loss, but your harmonics will be way down, the filter takes out ~ 40dB out band stuff.
The 3x3 mm filters are easy to use, the smaller ones are a bit hairy.

The pi-filter (band-pass) on the antenna is not very effective, and has a 2dB loss with ideal components. A simple low value cap (3pF NPO ~0.08dB S21 at 2.4GHz) ) may be enough to cut out lower frequency stuff, and block DC.

Bypass caps on the PA chip could be closer, the lowest value cap here at least. Why not pour ground around the whole top? More ground vias is better, too many is not possible!
Cream layer shows no paste under PA.
The nRF24L01 has a metal slug, I think this needs to be soldered in too, but the mfg. should perhaps be asked.

It is hard to inspect solder under the chips (w/o x-ray) but more solder would not hurt, the excess will be sucked out in the vias.

The DC blocking cap can be almost any value, just big enough to not attenuate the RF, 3 - 100pF should do. You can probably cut the trace and scrape off some solder-mask with an X-acto blade and shoe-horn a cap in the TX-line.

The thru hole USB may take less room than the one you now have. Micro USB is becoming more common, phones and stuff, and may save you some space. It can be hand soldered on the "other" side too.

I did not catch the shield mfg. but Digi-Key has those good'n cheap Laird parts with removable lid. the 32x32mm 903-1053-1-ND could work if you moved the RF connector to the "other" side, the 1x1" may be too tight.



I found the harmonics filter in the app note www.bocon.com.cn/artupfile/2013-12-24/02013122401460816545.pdf



www.mouser.com/ds/2/400/DEA162450BT-1288B1-269740.pdf probably better than the discretes, ~ 1 dB loss.

Any plans to include FASST?

Nordic Semi answered that grounding of the center pad is not necessary, nor possibly harmful:-)

The FAAST receiver I have here uses a www.rfmw.com/PortalPartSearch.aspx?txtSearch=ML2730 chip. It may already be "old".
I don't have a SPI bus analyzer so can't give you any dumps, but I'm interested to see how the "bind" works. Is it usually, or always, a two way hand shake? I would think the TX GUID is visible in the receiver SPI data stream? In one case the frequency hopping table was an algorithm based on this, but I guess it also could be a programmed look-up table or a dump from the transmitter?
I'm thinking of getting a Salae SPI bus analyzer, but they are not currently shipping,(new models underway) is that the one to get?

The PCB could use some more vias, the output connector grounds will be more robust with vias, The PA chip in the app note has more vias (9), likely for thermal reasons. Cram in as many as you can.

A shield can around the TX may not be necessary, it is often included as an option in case you get into trouble.

mini USB thru-hole will save a little space, if needed, and micro USB thru hole even more.
Approximate board areas, 47 mm^2 micro TH, 71 mm^2 mini TH, and 89 mm^2 for mini SMT.
www.digikey.com/product-detail/en/ZX62D-.../H11610CT-ND/1963859

Personally, I don't think the surface mount USB connector is a bad choice. They're strong enough given how infrequently it's used on this module, they're quite easy to source, and if this ever gets mass produced, they can be placed for reflow soldering. That corner of the board isn't particularly busy, so the smaller footprint isn't really an issue.

Well, my boards arrived today. One of them has a power to ground short like yours, but the other two appear okay.. We shall see.


I got the top side mostly populated this evening. I ran in to one issue... I have no idea where I put the damn PAs when they arrived. They weren't in my bin with the rest of the parts. I went ahead and populated the top side anyways.. I'll use my hot air gun to place the PA when (if) I find them. I've ordered more just in case I accidentally threw them out with the pile of packaging.


Here's one fresh off the hot plate. I prefer the hot plate to the oven for this kind of thing; The only trade-off is you can't reflow a double sided board with it. I had planned on doing the back side by hand anyways. They turned out fairly well, only a few spots will need touchup. There are a couple of solder joints that are a bit dry due to having vias in the pads, which wicks away the solder. Easy enough to touch up.




Overall, they go together quite easily. It's nice to see that you didn't use the built-in 0402 footprint from Eagle, which has pads that are a little bit too big and far apart for good reflow. I'll look at cutting the trace and adding the DC blocking cap when I do the touch up.