Can you check over this DCSSR?

P

Ponddude

New member
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!
 

Attachments

  • small dcssr.pcb
    13.3 KB · Views: 61
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
 

Attachments

  • DCSSR.pdf
    211 KB · Views: 118
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...
 
Last edited:
  • 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
 
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.
 
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))
 
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.
 
Ponddude said:
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.
Click to expand...

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!
 
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.
 
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/Produc...irtualkey68900000virtualkey689-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...
 

Attachments

  • DCSSR 1.3.pdf
    108.8 KB · Views: 43
  • small dcssr.pcb
    11.5 KB · Views: 7
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.
 
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.
 
Matt_Edwards said:
For one last challenge, this should be able to all be done in single layer.
Click to expand...

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.
 
Matt_Edwards said:
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.
Click to expand...

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
 
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?
 
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.
 
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...GAEpiMZZMsh%2b1woXyUXjwVSLknFYNuvXAHpMTk16Mk=

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

Greg
 

Attachments

  • DCSSR 1.5.pdf
    109.2 KB · Views: 20
  • DCSSR1_6c_1250824655.sch
    123.8 KB · Views: 6
  • small dcssr.pcb
    11.8 KB · Views: 6
You must log in or register to reply here.
Back
Top