Hey guys,I'm an undergrad student from BITS Pilani,Goa campus,heading the on-campus CUA Initiatives.We're trying to build a custom PSoC3 board,to better suit our specific needs and for wider exposure of this tech amongst our student body.

The first version is going to be a bare-bones solution,i.e just the PSoC3 chip,the required capacitors around and a programming header,with as many pins broken out to headers as possible.All power rails will be provided via off-board supplies,or not.Lets see.

A few specs the board needs to meet,( I do understand these might be impossible to meet

1.Single Sided

2.Can be etched using toner-transfer method of self PCB Fabrication.(Hence the first point)

3.Can be hand soldered 

4.Low Cost.

All these point toward the DIY nature of board production and assembly,essential for easy access to PSoC3 solutions,without requiring large numbers of FTKs and DVKs.

Let me discuss each part of that in some more detail,since I want some help on this design.

The PSoC 3 Chip - Owing to the fabrication constraints mentioned above,we're going to go with the 48pin SSOP chips of the PSoC3 family for our initial designs. We would like to go with the CY8C3866PVI-021 (most feature rich SSOP part) but its $14.So,our next option is the CY8C3246PVI-147,which is priced at $7.We do lose a few features,but lets see how that goes.

.

Just the required capacitors - We'll probably have 0805 SMD caps where needed,according to the schematics(I'll come to that) in the datasheet for the PSoC3 Family.

.

Programming Header - Now this is the tricky bit.We would like to reduce cost and parts,hence the mini prog would be the first to go.That leaves us with 2 options,one - build that FX2LP programming circuitry OR,do a one-time program of a custom UART/SPI bootloader. The latter is more attractive,since it goes along nicely with our aims on this board(Simple to build,Cheap and widely useable).I have been following some topics here on the forum in this regard,and hope that this can be implemented.We do have old miniprogs from our PSoC1 kits,Could those be used to burn on the bootloader? ..Or is the new MiniProg3 absolutely necessary for that?

Power - There are lot many power rails than conventional controllers,so each of these will be broken out to a header(on our first fab).Adding some LDO voltage regulators etc will be a plan for the future,since as of now,the aim is to get a basic programmable platform.

.

Schematics - I'm not too sure on how the older MiniProgs(I2C ones..) can be used to program the psoc3,so I'm a little hazy on those details.If someone could clarify the chip's basic requirements with respect to programming etc for this initiative,I'd be greatful.

Comments,suggestions and criticism are most welcome on this.

Basically need some input on the real-world feasibilty of the above described design.

.

We'll try and have it be prototyping friendly(shields like the arduino,breadboard plugin-able without too much space loss etc) too,but I think thats too many design demands for a day :)

Hey guys,I'm an undergrad student from BITS Pilani,Goa campus,heading the on-campus CUA Initiatives.We're trying to build a custom PSoC3 board,to better suit our specific needs and for wider exposure of this tech amongst our student body.

Hey,

I dont have a lot of experience with fabrication,but I'll manage well,since I am experienced with the design end of it.

Yes,looks like a single sided board will be difficult to pull off,especially since I want to make it breadboard plugin-able(which means it cant take up lots of space on the board).Anyway,thats a later thing,since I will be prototyping this idea with a breakout board on a breadboard with associated caps and a miniprog to fire in the bootloader.

As far as the schematics go,I'm drawing them up tonight,and have opened a design review case for the same.

Only point I still need some clarification is the USB bootloader.There was an appnote, "USBFS Bootloader for PSoC(R) 3 and PSoC 5" which I cant seem to locate presently.

If the bootloader works out,(by works out I mean,the chip as well as PC side sofrware) then this board can be a really attractive prototyping solution for students and engineers everywhere,since the cost wont exceed Rs.500(USD ~10).While it is by no means a replacement for the awesome FTK/EVKs,but it can definitely make this great chip more accessible.

As it occured to me the other day,I'm trying to Arduino-ize the PSoC(in terms of hardware...) 

As part of later additions to this design,

-we could have boards bootloading each other(like the appnote that shows a 5 doing so to a 3),which means you'll need only one miniprog3,for the very first board :)

-Though USB Bootloading is very attractive not only for the low cost and super short BOM,it does cut out the debug features you'd get via SWD or JTAG.However,theres still USBUART(on board options..else an LCD or any other output peripheral is super easy to use with the PSoC),which is good enough for most projects.

hello

i plan to do similar than you, but i am fortunately emplyed to a company, and we should

deliver quality electronics to our valued customers which results in 4-Layer FR4 NiAu-plated..

but for prototyping a set of DVK 001 is at my hand, but they should not leave the lab.

for testing the programmed firmware in real environment off the lab i like to recommend a tiny schmartboard.

(www.schmarboard.com modell# 202-0011-01 rev B)

the granted me a free sample o a tqfp 32-100 0.5mm pitch board. excellent for

handsoldering the "big" PSoC3 parts since improved solderstop mask is on the pcb

and lot of pads for mounting 0805 caps on both sides . each pin is outlet to 1/10" raster and fit to drill board.

i personal, would not miss my miniProg3 for programming (fast ) and debugging,

so the 10pin SMD header is also in my design but from different vendor than DVK part (lot cheaper)

if additional electronis should be employed to your project and additional PCB space is need,

plug your "DIY processor board" onto your PCB, but strongly recommend double side.

even if you can process single side only, make excessive use of the groundplane.

( you may take a look to some older ham-radio  VHF projects, doing so for years..).

just a few thoughts concerning about the topic  "building a cheap but well working

psoc3 equipment".

good luck and greets from germany

Markus

Many thanks for the inputs,markus68.

Your post raised another doubt,regarding speed of programming via USB Bootloader.Will need to look into that too..

Also,does anyone have a copy of that USB Bootloader appnote? "USBFS Bootloader for PSoC(R) 3 and PSoC 5" , If so,please share the associated code and pdf.

Another thing I just realized is,I will need to go with the CY8C3866PVI-021 part,since the cheaper CY8C3246PVI-147 doesnt have USB! :P

Attaching the USB Bootloader Example that was originally available on Cypress website. Currently it is being totally revamped and possibly everybody can have a complete USB Bootloader soon(We request your patience until then  ) !  Arduino-ize the PSoC(in terms of hardware...)? Interesting. Probably you can come up with a PSoCduino !

Project and document attached now.

Attached is a picture of the (home) etched form of the breakout board for the Cy8C3866PVI-021.

Also attached is the pcb layout in pdf,incase anyone would want to take a shot at etching one for themselves.They are all 8mil tracks.

Just for Info,the software used to create this was Fritzing,and not something more professional like eagle or altium,since I'm still working on the creating the Cy8C3866PVI-021 part for them.(which is super easy on Fritzing,since they already have a 48pin part,just need to edit an SVG for the schematic symbol)

Sorry for no updates on this...was busy organizing this semester's PSoC1 Lecture series,and then tests(doing my masters in chemistry) came along(still on).

Will add more as soon as I get free.

But otherwise,

I've

0.made the breakout

1.recd the chips

2.Almost done the schematic

Great going !

Thanks U2 :)  ..About the schematic,

I've got a few points:

I've taken the datasheet's(CY8C38) entry on Power System(Page 29) as my reference for the various capacitors required.I also consulted the schematics of the FTK and the DVK(I'm talking about the CY8CKIT-030),and a Cypress Appnote on Decoupling Capacitors.

I have a few points I'm confused about,

1.The kit schematics use 0.1uF and 1uF across VDDd and VSSd lines,but the datasheet simply recommends a 0.1uF. ??

2.For the USB connections(D+,D-),

the PSoC 3 FTK uses direct connections to the chip,

the 030 uses a couple of schottky diodes,

the CY3124 EvalUSB kit uses series resistors,

the CY3209 uses the SN65220 in addition to series resistors.

Other designs,(PIC,Arduino etc) use 2 3.6V zeners,or direct connections.

Since I want to keep the design simple,yet not crude,which one do I go with? ..Are series resistors good enough? Or the zener arrangement?

3.Power levels- This isnt a world-ending decision,but I'd like to hear your guys thoughts on the power system on this thing.(USB or External or both? .. 3.3 or 5?)

 1.The kit schematics use 0.1uF and 1uF across VDDd and VSSd lines,but the datasheet simply recommends a 0.1uF. ??

2.For the USB connections(D+,D-),

the PSoC 3 FTK uses direct connections to the chip,

the 030 uses a couple of schottky diodes,

the CY3124 EvalUSB kit uses series resistors,

the CY3209 uses the SN65220 in addition to series resistors.

Other designs,(PIC,Arduino etc) use 2 3.6V zeners,or direct connections.

Since I want to keep the design simple,yet not crude,which one do I go with? ..Are series resistors good enough? Or the zener arrangement?

As per USB 2.0 Spec, for a USB FullSpeed device it is necessary to have 45 Ohm termination on each of the D+ and D- lines, to provide an effective differntial impedance of 90 ohm. The USB driver in PSoC3 requires the impedance on the bus to be between 28 ohm to 44 ohm and it is recommended to put a series resistor of 22 ohm on D+ and D-. The impedance on the line is required to be between 28 and 44 ohm including the series resistors. Hence the answer is to use 22ohm series resistors on D+ and D- lines.

The VOH signal for D+ and D- lines is 3.6 Volts. In PSoC3, there is an internal regulator on the USB bus driver which takes care of it, hence we do not need any external diodes. In Arduino and other AVR devices, the zeners are put to limit the D+ and D- signal levels.

3.Power levels- This isnt a world-ending decision,but I'd like to hear your guys thoughts on the power system on this thing.(USB or External or both? .. 3.3 or 5?)

It is always advisable to have an external power and USB as well. This was it is possible to have supply from USB. When the board requires larger current the preferred source would be an external adaptor or similar source.

I've done the first schematic,and posted it on my blog,

Image link here - 2.bp.blogspot.com/-6Vfj47P668Q/TnsXBv1GClI/AAAAAAAAAUU/1Le8MD4he4E/s1600/PSoC_Custom_Board_Rev1.png

A few points -
1.I've blatantly tied VDDd and VDDa together,at the VBUS of the USB port.I think I'll be changing that very soon.
2.Same for VSSd and VSSa.
3.Also,except for maybe a voltage regulator for the 3.3V level,I'll stick to this.
4.This work is licensed under a Creative Commons Attribution-ShareAlike 3.0 Unported License.

Attached is the EAGLE schematic(with the cypress_mod.lbr with the concerned chip,a custom part that I made) I've put together.

Mixed signal PCB design is something I'm finding hard to wrap my head around,but I'm reading hard on it(when I can).

I've tried to adhere to the "rules" of mixed signal design,and the guidelines in the Datasheet,regarding decoupling capacitors.However,I'm not able to conclusively decide where the ground planes should be.(Since theres no "exclusive analog half" and "exclusive digital half".Its more like digital(USB part) then analog(VDDa and Port 1),then Digital again(remaining right half of the board)..

Below is a shot of the board with VDDa and VDDd highlighted,to show you the digital and analog sections of the board..

So, 2 questions :

1.how would thr ground planes come up?

2.Is it ok to route USB signals "one on top of the other" (one in top layer,the other exactly below it on the bottom layer)

If youre interested in the PCB files,drop a comment below.

I know,there are a few obvious routing errors up there,I'll fix those.

Also,is this an excessive number of vias? ..or is that "ok" ?

I should also probably make the "power" tracks thicker.

I've done a second version of the PCB,changes include:

-addition of a 3.3V Power regulator and a power level selection jumper.
-Ext DC Power Source connector.
-widened all power tracks to 40mils.
-shortened USB tracks,since long high speed tracks add noise.
-added a 5 pin power header(Vin,Gnd,Gnd,5 and 3.3V).
-added an external pullup to XRES,since the internal one is weak.
-fixed the header alignment.
-and a few other routing and placement errors.

Heres a shot of the PCB:

Heres a shot of the PCB,rendered in 3D:

TODO: -Work on the silkscreen -Decide the ground plane(s) layout -Run a DRU,pre fabrication.

Sorry about the gigantic images.Too bad I cant edit my posts :(

I dont have much experience with the type and variety of SMD parts available,and thats the only reason I've used through hole parts where unsure.I'll revise the design soon to a completely surface mount board(except headers,ofcourse).

If I do plan to take this to commercial mass production,I'll go with 6mil tracks,and make the SMD parts like 0603 or even smaller,and use a fab house in china or similar.

Another point,

I've heard that the XRES needs to be 'OR-ed using a diode when its going to be connected to a programmer.Is this really needed in my case? Because the only time the XRES pin will be used as an XRES pin will be for burning in the bootloader.

When you have multiple source that will reset the PSoC device via XRES, it might be necessary to use diodes to seperate them. However if programmer is the only agent that will be applying XRES, you dont need to have a diode.

 Thanks U2..I really appreciate your taking out time for this thread,dispite your heavy work load.

 From what I've read about Mixed signal PCB design,I shoud have one continuous ground plane in the bottom layer.Could someone confirm this?

I'll also probably swap the 0 ohm resistors(linking the VDDd and VDDa) for ferrite beads or similar. 

 I'm currently in talks with various PCB manufacturers about the cost and specifications for the initial prototype boards.

Also,I'll publish a revised design soon which shall have all SMD parts,and will be production ready at any fab house.

I've made a few more changes to the design,with the goal of simplifying it,and decreasing component count.

-Removed the external DC jack.

-Removed zero ohm resistors,and added solder jumpers(from SparkFun's eagle library).

-Added the ground plane,which is of the "GND" net.(GND net is the USB's ground,shorted with the VSSA and VDDA using a solder jumper.)

-Changed the type of USB connector,since I had a bad experience with a miniusb one.Too small to comfortably solder,with an thick iron like mine.



And yeah,I've decided on a name - "EzPSoC3".

I'm waiting for a response on a case,on basically if my ground plane is "ok".Heres what the board now looks like.

Heres an image of the PCB - 2.bp.blogspot.com/-tchnaujm-YY/To3btSUeT_I/AAAAAAAAAUs/NJLAULhN3Bc/s1600/PSoC_Custom_Board_Rev5_OCt06.png

I've attached a pdf of the current schematics.All tips,guidance,suggestions and criticism are welcome.

kmmankad,

clean job !

keep it up !

-dave

Hey all,sorry for the sudden pause in progress and updates.I couldnt devote any time due to exams.Free from those now,I'm attaching the schematics and board file(along with the custom library,which has the PSoC chip and the sparkfun library as well as sparkfun DRU file),both with the ERC and DRC giving no errors.

Comments,suggestions,criticism and edits welcome

This work is licensed under a Creative Commons Attribution-ShareAlike 3.0 Unported License.

Sorry,forgot to attach.

PSoC3 Custom Board Schematic Rev6 - as on Oct 26.
This work is licensed under a Creative Commons Attribution-ShareAlike 3.0 Unported License.

Not able to attach files here,dont know why.

heres a link www.psocdeveloper.com/forums/download/file.php

More changes,and the board seems ready for the first prototype.

Heres a link on the latest :

http://www.psocdeveloper.com/forums/viewtopic.php?f=42&t=8096&p=36776#p36776

Heres the latest,pre-fabrication version of the board which has been Design-Rule-Checked using the DRU files from SparkFun as well as the popular PCB service,'Fusion' from SeeedStudio( http://www.seeedstudio.com/depot/fusion-pcb-service-p-835.html )

I've also added a few extra vias and features to allow for home etching of this double sided board,for those who can.

Further plans for the hardware include a through-hole version and an ultra-compact version(speaking of compactness,current dimensions stand at 2.7"x1.9").

I'm also updating this(dangerousprototypes.com/forum/viewtopic.php) post with the board progress.

Quick Update: I might have finally found an affordable source for the PCBs.Finalizing the details with him,and I hope to get the prototype boards soon :-)

So what will be the cost of the final board ? Approximately ?

Currently I'm planning to purchase 5 boards,so that comes to around Rs.1300 for me.But I hope that can be reduced,since I dont want soldermask and silkscreen,since this is only the prototype.But say around 250/board and then add to it the ~$14 for the chip and some more for the caps and other components,so the price might reach Rs.1000.

Something just occured to me,would I compulsarily need an external 24 Mhz crystal to use the USBFS component?

For PSoC3 production version, it is not necessary to have a 24MHz crystal for USBFS component operation. The internal IMO can be set to 24 MHz and used for USB clock. However for PSoC5 it is required to have an external 24MHz crystal if the design has USBFS component.

Great to know that unlike the microchip's pic/atmel's atmega series,the PSoC's internal clocking system is robust enough for USB applications.

Hi, I am new to this discussion but the work done seems to me remarkable. To my knowledge not using the quartz for clocking may compromise the use of RS232 communication, that may be a limitation. Moreover, why not to include anyway the possibility of using the miniprog 3 programmer? These two additions have a very limited impact on the cost of the board but make its use broader.

Ops, found programmer connector top left, is that right?

 The IMO of PSoC5 is 1% so should be good enough for UART function. But you do need crystal if using USB. The PSoC 5 however needs to have crystal as the IMO is not as good as that of the PSoC3,. We have a prject using the pSoC5, according to the old spec. it should be good enough , but have to change to a new PCB because of the change of specification of the IMO. 

• Most of the high speed communication component demand for high speed clock. In PSoC3 USB, the bus clock intelligently syncs to the USB clock and thus maintains the required tolerance for reliable operation. 
• In case of UART, if data is being sent or received at high speed contnuously and if there is any clock tolerance, it might affect the operation. Transmitting data in bursts instead of a continuous stream might help mitigate the issue. Having two stop bits instead of one will also help mitigate the issue.

gve,

The programming connector is on the top right of the board,into with the 5pin end of the MiniProg3 should be connected,for programming via SWD.(atleast,thats the intention :P )

After thinking about the design a whole lot more,I'll be changing a good deal.So,I've pulled back the fabrication order.

Things I want to change:

1.Add a 24Mhz crystal.Even though the IMO is good enough,a robust design should have a crystal.

2.Use 2 row male headers rather than the current single line form.Thats just more compact.

3.Re-work the whole power supply section.I wasnt very satisfied with it in the first place,the reason being that I am not confident about the LM1117-3.3V and associated electrolytic SMD capacitors being available locally.So I'll just go with a through hole LM317 and a fixed resistor setup to get to 3.3V.

4.Get the P1's unrouted pins out.If I add an external crystal(and say RTC one too,) then I lose a total of 4 IO pins,and I dont like that.So I'll squeeze stuff and try to get the currently unrouted pins(5) from P1 out to compensate.

5.USB Connector.I miniusb one would be ideal,but needs better soldering equipment than I have.But then probably even the SSOP part will be a problem for me.(the best christmas gift ever would be a DIP packaged PSoC3 part :P )

6.Other stuff like mounting holes,and any other suggestions you guys might have.

So I ripped up everything,and started from scratch.Heres the end result.

I really gave a lot of thought to the power supply section and tried to think of a lot of schemes which would be idiot-proof and would still be flexible.However,I decided to drop those thoughts,since the routing was getting really messy.

Finally,the board is summarized as below:

1.Chip: CY8C3866PVI-021

2.Power System:

>From USB - 5V,3.3V

>From Unregulated DC Vin - 3.3V ...it is also possible to provide unregulated input directly to the chip,w/o any regulators in the way(just connect the source to the middle pin of the power level selection jumper)

3.Form and features:2.1"x2.2" and the headers are exactly 1.7" apart,so its breadboard compatible too.Tight routing and placement makes this a very compact design.

Suggestions and criticism are welcome. :)

 As far as the crystal placement is concerned, it is always recommended to place it as close as possible to the PSoC3 part. You should also have crystal phasing capacitors and they should aslo be as close as possible to the crystal and the PSoC part. The trace lengths from the crystal termial to the PSoC pins should be of equal length. These are some of my immediate  observations. 

Similarly make sure that the lengths of the D+ and D- lines are almost similar, few mm difference should still be fine for Full speed device. Possible 22ohm series resistsnce should be put on each of D+ and D- lines.

 Please read the following App Notes that can act as a guideline for hardware design consideration and checklist before you go for another spin,

•  AN61290 - PSoC® 3 / PSoC 5 Hardware Design Considerations 
• AN54439 - PSoC® 3 and PSoC 5 External Oscillator 

Thanks U2! ..I'll surely go through those before placing my order.Development on this is going to stagnate again,since I have my semester end exams fast approaching :(

Here are the latest revised PCB files,checked by DRC files from Sparkfun,Seeed and Itead,so that shouldnt give you any trouble.

Feel free to modify the design to suit your needs.

This work is licensed under a Creative Commons Attribution-ShareAlike 3.0 Unported License

The PCB(brd file) looks great. A combination of the EZPSoC3 with the FX1 based programmer that you guys have put together should be brilliant. With shileds(daughter baord) for this board, it will be a killer.

Thanks for the support and encouragement,U2 :) Really makes my day ..

One thing though,someone over that the PSoC Developer forums has expressed that the USB Bootloader doesnt run when the chip is powered(all power lines) at 3.3V. I havent looked into it personally yet(I think it could be fixed in code,but need to look deeper..),but any ideas on why this could be so?

Heres the forum post from PSoCDeveloper forums : www.psocdeveloper.com/forums/viewtopic.php

Oh wait.This sounds like a straightforward fix.Looks like the code depends on the voltage configuration in the DWR,and setting that at 3.3V will start the USB component at the same,and all will be okay...

Its a simple software fix, don't worry about that. 

So I'm free from semester exams,and made more changes to the board,and sent them for fabrication.

-Changed USB routing to comply with guidelines in the USB design spec.
-Decided to remove the external Mhz crystal(but kept pads for a though hole resonator,just for testing)

(You may read a detailed writeup on those changes on my blog http://kmmankad.blogspot.com/2011/12/psoc3-custom-board-usb-routing-and.html)
And,sent the boards for fabrication(to a local guy) which I should get within a week of my sending,i.e around the 19th..

There is still a lot that can be changed and made tinier,but the current decisions in parts and their packages are made on the basis of my confidence in their local availability.As I hit the streets for parts soon,I hope to broaden my know of the components available,so I can incorporate them into future changes.
If you have affordable access(read no shipping or heavy import duties) from parts sourced from places like Mouser,Digi-key etc,feel free to use that luxury to better this board's design and layout.

Is there any reason why you are not using usb mini-B connectors? that would take less space and yet be easier to solder.

 Well,this is my first time doing SMD,so I'm not that confident with mini-B type of connectors...Plus,the D+,D- lines were crossing(if I recall corrrectly)..so layer changes etc were needed.If this design goes well,then thats something I'm definitely going for.

Thanks though :)

Current Status: Waiting for PCBs to arrive,and trying to procure 22R in 0805.

Greatings! 

I've got a problem with PSOC3 power on from USB. When i'm  pluging in USB cable nothing happens, but all power and groungs are presend, after repluging cable in 0-3 seconds PSOC starts.

Can someone tell me what is the problem, and how to fix it.

custom board, cy8c3446axi-99.

Regards Alex C. 

 This is kinda off topic,but anyway,I think the issue on your board is that of rise times.I  mean,the caps on the power pins.They should be according to the scheme on Page 29 of the PSoC3 Datasheet.Also consult schematics of existing kits for the the values of the caps.

Hope this helps :-)

back to my board updates,

I expect the boards tomorrow,after a few days of delay.I'm still many components short,(22ohm in 0805 is something no one seems to keep locally,and the SMD LEDs.)

But I think have enough to get it accepting programs,so lets see how that goes.

For future revisions' PCB orders,(if I still have any hobby budget left),I'll try SeeedStudio's Fusion service or ITead's service.

Just recd the gerber files from the PCB manufacturer.They look great! :-)

Cool...SeedStudio is a great way to go. 

 The PCBs are in!

I ordered 5 of these for a total price of INR 1100.I've started populating the other 4 boards,leaving this one for the pics.

A few things,

1.I shouldve got soldermask done too: But then I was told that the setup cost would be ~INR 1000,so it was a no-go.

2.I shouldve used a temperature controlled thin tip iron: Well,what happened was,the iron overheated at one point,and burnt out a few tracks(completely,so they came off) on 2 boards,so I've lost those tracks.I'm really pissed with myself about that.

More pics as I continue working on them!

For more pics and posts on this,you may head over to my blog, http://kmmankad.blogspot.com

 While this is all good,I'm wondering about the future of this project.

Issues on a a couple of fronts:

-Board Fabrication:I can go with Seeed,but that will require further investment.

-Even if I do get boards fabricated,it will be too costly for me to buy PSoC3 chips(I'm using free samples currently)..at almost $15-20 per chip.

-Procuring other parts isnt easy either,so that adds doubt.

Any ideas?

Seeing as the chip has a price of almost USD 20,and an MOQ of 60,combined with fabrication costs and prices for other passives,it doesnt look like this board can be "low cost" in anyway,if at all  there is someone who chooses to purchase these over cypress' own boards. 

 from where I stand.even if this isnt financially feasible to fulfill the goal for which it was designed,it was(is) still a very enriching pursuit.

The board works,no issues at all :-) I dont have access to a camera,so I cant upload any pictures,but the USB bootloading,programming etc,all went flawless from the word go.

 That is awesome news. Could you make a video of the same and upload on youtube. We would love to see it !

Inspired by my inital success with the EzPSoC3 board,I developed yet another board,the kind that isnt good in terms of analog noise etc,but serves as a low cost entry point to PSoC3.

I hooked it up to the miniprog,and programming it was easy,and seconds later,I had it accepting project files over USB :-)

More here http://kmmankad.blogspot.com/2012/01/psoc3-hardware-quick-and-dirty-fab.html

Pictures of the EzPSoC3 board in its final form: picasaweb.google.com/kmmankad/EzPSoC3

Pictures of the QuickPSoC3 board in its final form: picasaweb.google.com/lh/photo/QQc7ldVI0ossHO4OJNFHV9MTjNZETYmyPJy0liipFm0

I needed some PSOC3 Boards so I decided to buld your EZ-PSOC board. But I was not quite happy with the USB connector so I took your schematic, made a few changes and routed it again from scratch.

Changes over the original EZ PSOC3

* Blade style design for easy breadboarding.

* Mini-USB connector

* XTAL instead of resonator

* Added a Barrel Power Jack, so it's now posible to power it with a wall wart.

* Simplified Power Selection. By placing a jumper on J2 it is posible to select to be powereb by VUSB, Wall wart or taking power from the bread board.

* Added 5 LEDs.

I Forgot to attach the eagle files.

kmmankad please give your board to any pcb printing company so that they can provide cheap pcb to student

kmmankad tell me where do i get the components for the board(cypress soc,usb headers etc)?