I'm going to try and re-name the discussion from the 'dead or dying' thread...
Making contributions to Leaf Labs
(29 posts) (5 voices)-
Rod
Membergbulber - two topics; 48 pin CPU on the boards in GitHub and getting the GitHub designs into the hands of people who could make contributions to a common platform.
I just tried to layout a single part in Eagle that would be a 64 pin STM32 with a 48 pin STM32 inside it. I don't think its possible. No room for traces to connect the pads.
It would be fairly straight forward to modify an existing design with a 64 pin part to use a 48 pin part (assuming there is no critical functionality lost with the pins removed, of course).
Does it make sense for me to do that for the MM4?
On the second topic, I might be able to supply a few operational boards if there is a desire. Presumably that would involve a shared financing model. I wouldn't want to get too far into me financing the boards on my own at this point.
In terms of building a two layer 0603 board, its not too difficult. One just want to make sure to put all the passive parts on first and then the silicon, and then the tall parts.
Posted 3 years ago # -
gbulmer
ModeratorRod -
I just tried to layout a single part in Eagle that would be a 64 pin STM32 with a 48 pin STM32 inside it. I don't think its possible. No room for traces to connect the pads.
I think it needs to be a single footprint, not two connected together. I think the design rules I have set up might 'go nuts' with two footprints.
I had hoped that Eagle 6 would let me make it, because it now supports 'arbitrary' pad shapes, but I haven't made any effort to find out.Thinking about it, it probably isn't worth the effort in the short term. It might take more than 2x effort to test two different parts, and may be nasty if there are any bugs.
I don't know what the best way forward on a 48pin-part-based board is. I want to talk to a few chums next week. We'll take weeks to get clear because some software is on the critical path. We might want to do a board ourselves as a little student project. I really don't know.
I wasn't talking (writing) about making two layer SMD boards, I was talking about putting SMD parts on both sides of a board. It was a response to you saying
I was inspired by sly's lovely hand layout and Eagle's total trashing of the auto-router in 6.1 and am seeing a simple (although with components on both sides) ...
Sorry if I misunderstood or confused you. While I know that local school children have made boards with SMD parts on both sides, it is more complex, and I'd like approachable boards if practical.
Posted 3 years ago # -
Put a package inside a package?! That's neat!
http://twitpic.com/8ev9dq
http://dl.dropbox.com/u/42394/stm32-48and64.brdPosted 3 years ago # -
Rod
MemberOn the 48 + 64 pin layout question... I now think it would be possible, but it would require 5/5 resolution with .010 minimum drill diameter. I'm not aware of an inexpensive, low volume PCB provider that offers that kind of resolution. Mine uses 7/7 with 0.16 minimum drill.
A pretty complicated layout for the nested chips.
It would be simple if they'd matched the centre pins of the the higher pin count package with the the pins of the next lower pin count package, but that's not what they have done. There is an offset of a pin position or two. So I think vias and connections on the reverse side are required to make the trick work.
On the two layer point, you now have me quite confused about the distinction between '2 layer' and 'components on both sides'. By '2 layer' I mean copper on top of the board and copper on the bottom of the board. It does make sense to keep the components on one side only if you can, but with the MM4 board the small size makes the board useful as a simple component in larger systems. I think the smaller size is a significant advantage and worth a little bit more trouble in soldering.
Posted 3 years ago # -
gbulmer
ModeratorRod -
On the two layer point, you now have me quite confused about the distinction between '2 layer' and 'components on both sides'.
Okay
By '2 layer'I mean copper on top of the board and copper on the bottom of the board.
Yes, that is what I mean too.
I am not writing about "components on both sides".
I am writing about "SMD components on both sides". By that I mean SMD components are soldered to the top of the board copper layer, and other SMD components are soldered to the bottom of the board copper layer. What do you call that? Maybe it is a terminology difference between the UK and the USA?The technique used at my local school to teach children how to make SMD boards is the "toaster oven" (low-cost reflow oven) approach where solder paste is applied to the board, parts placed, and the board heated. It works very well, fewer health and safety issues (vs 24 children using soldering irons) and the kids seem to enjoy it.
To put SMD parts on both top and bottom copper, the first side (say top) has parts both soldered and glued to the board. So the board is solder pasted, parts (glued) placed, and heated twice. This is doable, but it is quite a lot more time and effort, and more opportunity for things to go wrong. So I want to avoid using these types of designs with children and beginners.
It does make sense to keep the components on one side only if you can ...
This is a big issue to me for my target users. At the moment, I will avoid boards that require SMD parts to be soldered onto both sides of the board.
Posted 3 years ago # -
gbulmer
ModeratorRod -
On the 48 + 64 pin layout question... I now think it would be possible, but it would require 5/5 resolution with .010 minimum drill diameter.
Those constraints are too expensive. I might have another look one day, when I have plenty of spare time, but that is enough for me to put it "on the back burner".
Posted 3 years ago # -
Rod
MemberThe old toaster oven trick... Ok. That makes sense now. I will give that some thought.
I wouldn't actually rule out the 48 to 64 pin thing. If I was going to do it I would do it as an adaptor. A tiny little board that mapped the pins. It could be really cheap (like pennies) but the way I envision it it would have a via in the middle of the 64 pin pads, meaning that the hole would be in the middle of a 12 mil trace or would have to be 8 mil or so in diameter.
So maybe the thing to do is to see if there are some available on the web.
Posted 3 years ago # -
siy
MemberOut of curiosity I've tried to prepare single layer version of Mini. With some simplifications (no separate analog ground plane) and some additions (RTC crystal) I was able to put it into size close to original Mini - same length (51.3mm) but little larger width (21.3mm). Partially width is dictated by slightly increased pin header row pitch (0.6" is too tight, so I've switched to 0.7"). Since all components are at the same side, there should be no problems with reflow soldering.
I've made few PCBs and going to assemble one or two of them. If there will be no obvious issues I'll submit design into repo.
By adding second layer there should be no problems to add missing separate ground plane. Also, Initially I've tried to place MCU rotated by 45 degrees just like it is done in original Mini, but quickly realized that this is quite inconvenient for routing, so I've returned to traditional layout. I think that by adding another 0.1" to row pitch and some "stretching" this layout can be used for 64-pin packages too, but so far I have no plans to try this version.Posted 3 years ago # -
siy
MemberFiles are in my repo (https://github.com/siy/openstm32hw) and once pull request will be processed, they will be in main repo too.
Posted 3 years ago # -
Rod
MemberSiy I had a look at your mini48. Love your layout.
I would suggest a couple of smaller components.
The C&K KMR 2 series tactile switch is the one used on the Maple Mini. Its very nice and a couple of mm smaller than the 1101 from IL switch.
Also the Epson C-002RX 32K crystal in the 2x6 mm can we use in ton lots. Its a very good choice.
Posted 3 years ago # -
siy
MemberThanks, I was looking for exact part number of such switches for some time (I saw these switches at some boards). Unfortunately they are not in stock in local stores. I'll try to purchase them online, although this might take some time.
About crystal. I have crystals in 2x6 package, but I prefer SMD parts where this is reasonable. I've used KX-327LT part produced by Geyer just because it, probably, one of the smallest 32K crystals in SMD package available in local stores. Epson has identical part MC-146 which might be easier to obtain (DigiKey has MC-146 32.768KHz in stock, for example).
My main problem with such a cheap parts is that if they are not available via local stores (either in stock or by order), they are hard to obtain elsewhere for reasonable price because of rather expensive shipping. For example, Mouser charges minimum $50 for shipping in Ukraine via EMS (cheapest available option). This is no big deal if I'm purchasing something relatively expensive (MCUs, for example), but for $0.25 part, even if I order 100 items, this effectively triples the price of each item. And 100 switches is far far more than I actually need :)
By the way. I've tried to prepare Mini48 layout with 0.6" pin header row pitch. This is doable, but requires switching to 0.1/0.1mm traces/spaces. So far attempts to make such a board at home failed, but these attempts show that this is definitely doable, although (obviously) more tuning of process steps is necessary. Actually I can already reliably etch such a boards, but photoresist development process requires more tuning because resulting boards have bridges caused by not completely washed out photoresist.
Posted 3 years ago #
Reply »
You must log in to post.