PDA

View Full Version : Can you check over this DCSSR?



Ponddude
01-14-2010, 04:37 PM
Hi all,

I need to make several DCSSRs, but LabRat's and wjohns were a little to big for what I am looking for. I need something that is very small, or at least as small as it can be with DIP components. I created this off the previous versions of the COOP boards. Can you guys check these over and make sure they are ok? I would appreciate it!

budude
01-14-2010, 04:43 PM
Can you provide a PDF? I don't have the schematic prog on this computer...

51fordf2
01-14-2010, 05:12 PM
Can you provide a PDF? I don't have the schematic prog on this computer...

And/or tell us which program you designed it in...most of them have the .pcb extension, but don't play nicely with each other...

R

Ponddude
01-14-2010, 05:15 PM
Yes I can...sorry should have done that first...

This was made with the ExpressPCB software.

I am not 100% certain how to create a PDF direct from ExpressPCB, but I made one anyway.

Greg

budude
01-14-2010, 06:00 PM
Hmm - - what are your current requirements? What are the trace widths for the power/ground runs? They might be too small but would need answers to both. Your output on pin 15 of the Opto runs pretty close to the logic side - you may want to see if you can move that around assuming you want isolation.

You could put the resistors vertical vs horizontal to save a lot of space and provide more room around the opto to get those traces moved.

Another thing is the 5v regulator - if you switch to the LDO version (wjohn's can use either) you could save more space but it might depend on what you expect for an input voltage if the thing can dissipate the heat if it's a high V input...

David_AVD
01-14-2010, 06:44 PM
Schematic? Anyone? Anyone? :p
Regulator input is missing it's bypass capacitor
Insufficient track - pad clearances
Track for R9 - R12 double backs on itself
Regulator is sharing track with output drive

budude
01-14-2010, 07:01 PM
If your current requirements are low, you could look at ULN2803A drivers (doubled up outputs) instead of using the FETs and then you could really make this small! Only caveat would be that you need to invert the PIC outputs but that should be easy.

LabRat
01-14-2010, 07:12 PM
If "space" is the drive then consider removing LED1, or at a minimum reducing it's size from a 5mm to something smaller (perhaps even surface mounted?).

Are you planning to home etch? Or send this out? If at home, then I think you need to re-visit some of the spacing as the traces (in some cases) are very close to the pads.

Why run the "common" trace from the RJ45 to the "bottom" end of the stack of the row of resistors? you could shorten it and simply connect it up to R9 (vs R12)

I would recommend at least one (possibly two) more rounds of "go and clean up some traces). Getting rid of some of the right angles, looking at shortening some routings etc. (ex. Drop the 7805 a fraction lower, and the two traces going off to the right should align directly with the R5 and C1.. no awkward angled traces etc).

Post some pictures when you do the final board... I'd like to see the finished version.

(Afterthought - did you check the trace width calculator(s) to ensure your traces will support the desired current? (Something I learned about here on the boards... all my previous boards were never driving much current, so I never had to think about such things))

Ponddude
01-14-2010, 07:21 PM
Thanks everyone for the great input! I am going to go back and revisit all the points you made.

These are not going to drive much current at all. I am shooting for around 120mA MAX on each channel. It is going to be used for RGB matrix driven by the Freestyle...I hope. Still a work in progress.

RPM
01-14-2010, 07:40 PM
You could put the resistors vertical vs horizontal to save a lot of space and provide more room around the opto to get those traces moved.

SIP resistors can also be used to save board space.

budude
01-14-2010, 07:42 PM
Thanks everyone for the great input! I am going to go back and revisit all the points you made.

These are not going to drive much current at all. I am shooting for around 120mA MAX on each channel. It is going to be used for RGB matrix driven by the Freestyle...I hope. Still a work in progress.

If that's the case, then I would look at the ULN2803 - just a single chip replaces all those resistors/MOSFETs on the outputs and with doubling the outputs (since you can't use 8 anyway as-is) it would easilly drive your LEDs. The only issue with this is your use of the FreeStyle - unless you get RJ to cut a new version of code to invert the outputs it won't work.

Now - - you could drive an output into another input and then use the second output and that would give you a non-inverted drive and it would still have enough juice to drive your LEDs.

Besides everything else - a single ULN2803 will be cheaper than 4 MOSFETs and the resistors!

aussiephil
01-14-2010, 07:56 PM
If your only going to 120mA max per ch then swap to a TO92 packaged mosfet rather than the TO220, this will save lots of space.
Stand all resistors on end.

What's the input voltage? more than 12v then the 7805 may need a heatsink.

as RPM jumped in and said consider using SIP resistors.

Ponddude
01-14-2010, 08:25 PM
These ideas are great!

The input voltage will be 12 volts, so I don't think I will need a heatsink.

I increased the Trace sizes and moved the traces that were close to the pads.

I am going to skip the resistor networks, although a good idea, I may use these on another idea of mine, and don't want to be stuck with the limits of the networks.

I stood up the resistors and that saved a tremendous amount of space.

I also switched over to the TO92 MOSFET sizes. I think these should work...
http://www.mouser.com/Search/ProductDetail.aspx?R=VN10KN3-P003-Gvirtualkey68900000virtualkey689-VN10KN3-P003-G

I believe this version should work a little better and I have the size down to 1.5" x 2"...exactly what I was looking for!!

Let me know what you think...

Matt_Edwards
01-14-2010, 09:49 PM
Sorry I am late on this one.
I would:

Move the resistors R9 to R12 to the other side of the diode. that will free up track area.
Change the 7805 to a To92
Rotate the FETS by 180 degree so the Gates are closest to resistors
Rotate R1 to R8 by 90 degrees. this should get rid of a fair amount of duplicated track area as is
Add a small electro to the input


For one last challenge, this should be able to all be done in single layer.

David_AVD
01-14-2010, 09:58 PM
Looking better. You still need a 0.1uF capacitor between the input and ground of the regulator. Maybe add in just behind the DC input? Without it, the 7805 can become unstable and oscillate, sending the output voltage off and making it get quite hot even with little load.

Can you turn on a "45/90" degree routing mode in that software? That will help by only allowing nice corners and entries to pads. This makes for a neater layout and will be processed a little better by a PCB company as it's easier to spot stray tracks (from film scratches, etc) when the actual layout is neat.

David_AVD
01-14-2010, 10:03 PM
For one last challenge, this should be able to all be done in single layer.

Do you guys every do "design challenges" here? On another forum (micro controllers), sometimes someone will post a design problem with a challenge to see who can make the most compact (but correct) code.

Sometimes these brain storming sessions produce some real gems. Everyone using different CAD programs may make that difficult here though.

aussiephil
01-14-2010, 10:46 PM
Sorry I am late on this one.
I would:

Move the resistors R9 to R12 to the other side of the diode. that will free up track area.
Change the 7805 to a To92
Rotate the FETS by 180 degree so the Gates are closest to resistors
Rotate R1 to R8 by 90 degrees. this should get rid of a fair amount of duplicated track area as is
Add a small electro to the input


For one last challenge, this should be able to all be done in single layer.

Not sure i would change the 7805, only because it's a ubiquous part, inherently stable and there is still room on the board for it.


From the Fairchild Semiconductor data sheet footnotes for a 7805:

(2) Cin (0.33 uF) is required if regulator is located an appreciable
distance from power Supply filter.
(3) Cout (0.1 uF) improves stability and transient response.

i'd also rotate the fets 180

Aussiephil

Ponddude
01-14-2010, 10:54 PM
I screwed up on the board....the 0.1uF should be between pins 2 and 3 of the 7805. I also am not going to change that regulator, simply because I have a lot on hand...haha. I also rotated the MOSFETS. Do you think I should put a .33 cap along the positive input?

David_AVD
01-14-2010, 10:58 PM
Yes, put a small cap on the input. The recommended value varies a little by manufacturer (of the 7805). Somewhere in the 0.1uF - 0.47uF range should be ok. Personally, I'd have a small electro (47uF) there as well.

Ponddude
01-14-2010, 11:59 PM
Ok, a few more adjustments and I got it a little smaller as well. I put a .33uF electro cap inline on the positive feed, but for some reason it is striking me as wrong. Is there a better place for it?

Here is what I was thinking from Mouser...
http://www.mouser.com/ProductDetail/Nichicon/UKW2AR33MDD/?qs=sGAEpiMZZMsh%252b1woXyUXjwVSLknFYNuvXAHpMTk16M k%3d

I also am attaching wjohn's SCH (hope he doesn't mind) as this is what I was going off of.

Greg

David_AVD
01-15-2010, 12:01 AM
Ok, a few more adjustments and I got it a little smaller as well. I put a .33uF electro cap inline on the positive feed, but for some reason it is striking me as wrong. Is there a better place for it?

Greg, the 0.33uF cap goes across the DC input, not in series with it.

Also, the tracks from the opto to the FETs can be smaller, which would give you much better clearances.

Ponddude
01-15-2010, 12:06 AM
I told you I knew there was something wrong...haha. I guess I am too tired for the simple stuff.

I also never changed the size of the traces after I switched over to the TO92 style. I'll get all of these changed tomorrow.

Thanks again everyone for your help!

Greg

Matt_Edwards
01-15-2010, 12:34 AM
Do realize the pin marked GND is useless to you? You can't use it to connecthte other side of you lights. The FET outputs switch your lights to GND.

David_AVD
01-15-2010, 12:37 AM
See, this is why I keep banging on about schematics!

Here we are looking at layout problems when a schematic would save all this revision. :)

budude
01-15-2010, 12:52 AM
See, this is why I keep banging on about schematics!

Here we are looking at layout problems when a schematic would save all this revision. :)

Pretty sure he just based it off the existing SSROz v1.0 layout/schematic.

David_AVD
01-15-2010, 01:00 AM
I must admit since I'm new here, I haven't seen many of the designs close up. Sorry if I'm jumping to conclusions.

There just seems to be a fair amount of people wanting to do their own versions of existing designs, but for what reason? Is there something wrong with the original circuits, or is it just for case size etc?

Matt_Edwards
01-15-2010, 01:04 AM
I agree with David's comments about schematics - they go hand in hand. See my hand sketch below. it can be done on a single layer but I have had to change the position of some components so your schematic will also need updating.

Anyway, this is just a suggestion so use it is you see fit.

Ponddude
01-15-2010, 01:26 AM
Ok, here are the PCB files and the SCH file.

RavingLunatic
01-15-2010, 01:44 AM
WARNING: Minor detour of the thread coming. Skip ahead if looking for technical info related to the OP.


I must admit since I'm new here, I haven't seen many of the designs close up. Sorry if I'm jumping to conclusions.


Since you are new to the community let me share a thought with you about how you interact with the rest of the community (especially since you have already had a rather negative encounter in another thread). You should approach your posts less from a "You are doing it wrong because its not the way I do it" and more in a "Here are some suggestions that might help you" frame of mind. Members are looking for help/suggestions not lectures.





There just seems to be a fair amount of people wanting to do their own versions of existing designs, but for what reason? Is there something wrong with the original circuits, or is it just for case size etc?

I think the name of the community explains it pretty well, Do It Yourself. Our members love to do things for themselves and create something that they can identify as their own. Most of the time there is clearly nothing wrong with the original circuit since they are basing their own design on that circuit and just changing the form/fit to suit their taste.

Most members just want some new eyes to look over the layout to make sure that there are no errors. Since they based it on an earlier design they don't feel the need for a schematic and those familiar with the previous design will be able to see how the new layout should work and be able to see errors/flaws. Is it the perfect way to do things, probably not but in an open community like this you cannot expect each member to use the same methods to achieve their goals.

So please try to be less critical of how someone is getting the job done and more helpful in getting the job done.



OK for those who wasted their time reading this, time to move along to the next post and help Ponddude with his effort.

David_AVD
01-15-2010, 01:50 AM
There's still a lot of problems to be overcome. The schematic show the opto LED cathodes going to +5V. I assume the SSR uses ground activated inputs?

The other issue is the opto pinout. The Vishay ones we use go:



A |1 16| E
K | | C
K | | C
A | | E
A | | E
K | | C
K | | C
A |8 9| E

Note that every second opto is reversed. You'll need to check that too.

This design business is trickier than it looks eh? LOL! :D

David_AVD
01-15-2010, 01:58 AM
Hi RL, Nice to meet you. :)

I'm having trouble reconciling your advice. You mention that it's DIYC and it's each persons right to do it their way. I completely agree on this. I'm sorry if you or any other member sees my input as lecturing. I see it as constructive criticism. Why simply state the solution when you can tell the poster why the solution fixes their problem? You know the tale about "teach a man to fish" and all that?

Maybe it's a cultural thing going on between certain members (including me)? I'd like to think I'm pretty forthcoming with helpful technical information. Do I have to? No. Do I enjoy helping others? Of course! :)

EDIT: Is it the avatar that's putting you off? LOL!

budude
01-15-2010, 02:21 AM
There's still a lot of problems to be overcome. The schematic show the opto LED cathodes going to +5V. I assume the SSR uses ground activated inputs?

The other issue is the opto pinout. The Vishay ones we use go:



A |1 16| E
K | | C
K | | C
A | | E
A | | E
K | | C
K | | C
A |8 9| E

Note that every second opto is reversed. You'll need to check that too.

This design business is trickier than it looks eh? LOL! :D

OK - of course I did not mean SSROz (which is AC...) above but simply wjohns DCSSR v1.0... oops...

The opto used from the normal DCSSR BOM is Vishay K847PH available at Mouser: http://www.mouser.com/Search/ProductDetail.aspx?R=K847PHvirtualkey61370000virtu alkey782-K847PH - it's a modular design so the pinout is the same throughout.

David - I can tell you from my side that I wanted to get back into etching my own boards again and used LabRat's layout to build them. His layout was specifically designed to fit a Keptel TA-200 enclosure and it's mounting holes. It was an easy one-sided layout so it was a good choice to ease my way into it again (after a ~30 year hiatus).

edit -- and yeah - it's that Avatar - - lol...

David_AVD
01-15-2010, 02:28 AM
I'd whip up the layout for you, but we only use Altium DXP and I don't believe it exports to Eagle, etc.

On some of the other forums my user title says "White n Nerdy!" LOL

EDIT: I think I know the optos you mean. PC817 and similar have that same modular structure.

Cheater
01-15-2010, 05:20 AM
Off topic - David when you say 'we', who do you mean exactly? :)

David_AVD
01-15-2010, 05:40 AM
Sorry, I should explain I guess. I own a small electronics company called Audio Visual Devices, hence the AVD in my user name. (I use that name on several forums)

When I say "I", I mean me (of course), when I say "we" I mean the staff of AVD. Sorry for any confusion. :D

n1ist
01-15-2010, 10:25 AM
Greg-
I just looked at the latest board. The things that I would change are:

- As mentioned, fix the polarity issues with the opto LEDs and change the output ground terminal to a +12 one
- replace the 90 degree bends in the traces with a pair of 45 degree ones
- Add some mounting holes
- Some of those backside traces are only spaced by 10mil. While I know that ExpressPCB can fab down to 8 mil spacing (and they even did 6 mil on one of my boards accidentally) that's a bit close for home etch. BTW, the only traces that need to be wide are the ones involving the FET drains and sources, so you could just reduce the track width and get the increased spacing for free.

/mike

Ponddude
01-17-2010, 11:40 PM
Ok, I was away for a bit, but am back on track now...I hope. I adjusted a bunch of things, mainly every thing you guys told me. These are going to run on 12VDC, so do you think a 50 volt .33uF Aluminum Electrolytic Cap will do the trick? Also, is that entirely necessary on the feed to the 7805 reg? I also have the other cap, which is a .1uF fixed. It comes out of pin 3 of the 7805 (output pin) into the ground feed of the board. I also adjusted all the bends of the traces to 45 degrees, at least the majority of them.

Can we also talk about the MOSFETs? I think these should work from Mouser...

http://www.mouser.com/Search/ProductDetail.aspx?R=VN10KN3-P003-Gvirtualkey68900000virtualkey689-VN10KN3-P003-G

...but my question is if 60ohms is enough to drive the 120-150mA of LEDs I plan on having on these beauties? I am fairly certain they should work but math was never my strong point.

I am fairly happy with the design, unless you see any traces or components that are wrong. Let me know what you guys find. I would appreciate it!;)

Greg

Tabor
01-18-2010, 12:17 AM
Withou being able to open up the pcb files, can you tell me the size of the board now?

Ponddude
01-18-2010, 12:25 AM
It's 1.8"x2.5".

David_AVD
01-18-2010, 12:28 AM
I think you'll need to find better FETs than those ones. The specs are a bit on the ugly side, especially the "RDS (on)" of 5 Ohms.

Maybe stick with the TO-220 packaged ones like the IRL510PBF. Still cheap, hard to kill, low RDS (on), 100V tolerant and logic level drive to boot.

Ponddude
01-18-2010, 12:39 AM
Hmmmm...I would like to keep them in the TO-92 package, at least for space they save.

Maybe this one is a little better with an RDS of 1.5 ohm...

http://au.mouser.com/ProductDetail/Supertex/TN0606N3-G/?qs=sGAEpiMZZMveMCOqFR6qCFJZu68LG%2fC0PV1RbXtBkcE% 3d

David_AVD
01-18-2010, 12:43 AM
Looks ok at a glance. The thing to make sure of is that's it's a logic level drive type, which that one appears to be.

aussiephil
01-18-2010, 01:16 AM
Pondude

I'd use
http://au.mouser.com/ProductDetail/Fairchild-Semiconductor/BS270/?qs=sGAEpiMZZMveMCOqFR6qCMvPDPdTj2JVUfOZsO6MVkM%3d

Lower Rds on at 5v and much cheaper.

Question on layout

Not knowing how box size but do you have enough room from the output connector to the box sides for the cables?

Cheers
Aussiephil

aussiephil
01-18-2010, 01:19 AM
Hmmmm...I would like to keep them in the TO-92 package, at least for space they save.

Maybe this one is a little better with an RDS of 1.5 ohm...

http://au.mouser.com/ProductDetail/Supertex/TN0606N3-G/?qs=sGAEpiMZZMveMCOqFR6qCFJZu68LG%2fC0PV1RbXtBkcE% 3d

The one i just suggested has a similar Rds at 5v and is 1/5th the price :)

cheers

David_AVD
01-18-2010, 01:21 AM
The one i just suggested has a similar Rds at 5v and is 1/5th the price :)

Cheap as chips..... err.... I mean FETs !! LOL

n1ist
01-18-2010, 10:36 AM
The trace from pin 4 of the opto runs quite close to the pad for R11. Likewise the traces from R3 and the pads from R7 (comp side is even closer than ckt side).

A few tips on the schematic:
- It doesn't pass DRC (file->Check schematic for netlist errors)
- I would add the output connectors to fix the errors
- All 4 sections of the opto can be called "opto" if they have different pin numbers

/mike