XS1-L4A-64-TQ48 Test board

XCore Project reviews, ideas, videos and proposals.
User avatar
AtomSoft
XCore Addict
Posts: 135
Joined: Mon Dec 14, 2009 3:02 pm

Re: XS1-L4A-64-TQ48 Test board

Postby AtomSoft » Tue Jan 28, 2014 8:47 pm

Whats the down side to leaving !MR on VDD?

JTAG and MISO/MOSI lines are straight from PDF / Datasheet so i assume them to be correct. But as usual i wouldnt mind a second set of eyes on this.
User avatar
mon2
XCore Legend
Posts: 1679
Joined: Thu Jun 10, 2010 11:43 am

Postby mon2 » Tue Jan 28, 2014 8:55 pm

Connecting the #MR direct to Vdd (+3.3 volt) would be acceptable. According to the datasheet it is safe to leave floating since there is an internal 90k to Vdd. Either way is fine.

However, you have it currently connected to SENSE (1.0 volts) - not good :)

Can you post your latest TOP and separately bottom layers of the PCB layout ?

See possibly some issues on the IDC header wiring (2 x 10). The pins oscillate top, bottom, etc. so you must be cautious of where is Pin # 1 on the male pin header block. Also, do you plan to use a straight up (veritical mounted) 2 x 10 pin header strip or will it be right angle with a key (like used on the Slice Kits) ?

Do you plan to have the IDC header with or without the shroud to prevent wrong direction mating with the external JTAG tool ?

Shrouded straight with 0.1" spacing:
http://www.hochien.com/2532.html

Shrouded R/A with 0.1" spacing:
http://www.hochien.com/2533.html

Note from the above diagrams on how pin 1 -> pin 2 -> pin 3 is mapped. You must be sure to follow this pattern as well to allow for the XMOS tool to operate as-is.

If you do want the shrouded version, you must leave extra elbow room. Is your Pin #1 marked on the IDC header through a square peg and/or silk screen ?
User avatar
AtomSoft
XCore Addict
Posts: 135
Joined: Mon Dec 14, 2009 3:02 pm

Postby AtomSoft » Tue Jan 28, 2014 10:23 pm

This is the latest... but i didnt remove the MR line yet... that will be done in a minute... as a note... the HEADER and Pins be it MALE or FEMALE will be on top side and all components on bottom. This allows for me to use a nice space for all the pin labeling.
You do not have the required permissions to view the files attached to this post.
User avatar
AtomSoft
XCore Addict
Posts: 135
Joined: Mon Dec 14, 2009 3:02 pm

Postby AtomSoft » Tue Jan 28, 2014 11:05 pm

I remember about the position on the #1 pin from the pdfs ive read... they say ensure GNDs face edge of PCB Which is what ive done :)

Side note: http://www.youtube.com/watch?v=lY7I2Qs4MIQ
User avatar
AtomSoft
XCore Addict
Posts: 135
Joined: Mon Dec 14, 2009 3:02 pm

Postby AtomSoft » Wed Jan 29, 2014 1:02 am

newer PCB design... Connector (xSYS) is further out allowing more space for actual connector. This will allow a Straight header or Right Angled...
You do not have the required permissions to view the files attached to this post.
User avatar
mon2
XCore Legend
Posts: 1679
Joined: Thu Jun 10, 2010 11:43 am

Postby mon2 » Wed Jan 29, 2014 6:55 am

The board looks very nice ! Perhaps consider to offer pads or holes to extend pins 17 & 19 of your JTAG header to allow for (optional) use of the RX & TX modes for UART to USB debugging.

(optional) - add a SMD led on the topside with a current limiting resistor to a GPIO pin to allow for a rapid test using code to flash the LED ? Nice to have a visual confirmation that the board is alive - we do this all the time with mbed code development.

Reference:
https://www.xmos.com/en/download/public ... 1.0%29.pdf
page 5

Be sure to correct the #MR pin on the TPS3808 - ok to leave it floating (if it has not been done already).

Do you plan to use standard 0.1" male pins with this adapter ? Please confirm the hole size for the PCB to suit your preferred male header pins. For example, one option is to consider machined pin socket headers like this style:

http://www.anytek.com.tw/EN/product_show.aspx?id=3258

We sourced ours from WAFE (China) for a similar strip of the above. Believe these pins will be more breadboard friendly vs. the standard 0.1" square pins.

The schematic is difficult to follow as drawn for the port pins to PCB holes mapping. I would suggest you draw and define the adapter board like a standard IC pin mapping convention.

So, as a suggestion, sync the schematic with PCB as follows:
Pin_1_PCB (use square peg for hole and/or mark on silk screen as square) = X0D25
.
.
Pin_13_PCB = Ground
Pin_14_PCB = X0D13
.
.
Pin_26_PCB = +3.3 volts

Do you plan to build these by hand will have an assembly house build them for you with automation ?

The only other small pieces of advice are for the production side of things..

1) Source FR4 RoHS compliant PCBs
2) Work with a UL certified vendor and request they place their UL mark + Logo (optional) with mfr date code. Soon you will have many projects and it will be difficult to sort out who the vendor is / was - trust us on this one :) Also to keep the vendor responsible for any QC, you will want their markings for your record keeping. You should also be sure the PCB is 94V-0 compliant (apply to the TSK or BSK) for the flame rating. If you market your product, that is often a min requirement by vendors and is a safety issue for most clients. Again, a truly UL accredited PCB shop will be fine with this request.
3) LPI glossy green solder mask is our preferred choice but to some, the glare can be a nuisance so at your option, consider the matte finish. Different colors are nice to experiment.
4) Automatic silk screening is preferred over manual for proper registration and sharp text for your TSK and BSK layers.
5) Highly recommend that you consider at least 2 corner fiducials to allow for SMT machinery to properly align the PCB into automated machines. Often they are diagonal to each other at the ends of the PCBs. Such fiducials (unplated pads) allow for the vision system to orient the PCB (jiggies with the X & Y) for accurate placement for say the TQFP on your design.
6) To assist with automated assembly, consider to panelize your PCB into multiple boards per panel. Perhaps 4-up or 8-up, etc. You will need to apply carrier strips to the edges that will be broken off manually after assembly. Remember that if you V-score the edges of the PCBs, they are very very sharp to handle. We prefer to have most of our PCBs routed for a smooth finish to avoid finger cuts. Some like to have small 'mouse bites' for break aways. It is a personal choice. If you need help with this, let us know and can share some panel shapes we use in house that have worked well over the years. Believe we are using 5mm carrier (left & right side) strips to shuttle in small boards like your size. The carrier strips also feature fiducials for alignment with the SMT stencil printer and/or SMT machinery.
7) Do you have access to SMT stencils ? We use Power Stencil (powerstencil.com) in Shenzhen - they are one of the best (highly recommended by mentors) in the industry and work with Intel, Samsung and many others. We do not believe we have the lowest cost for the stencils but the quality is mint and they have a staff that can advise on any pending issues. FYI, we are paying $ 150 USD for a framed 29" x 29" stencil (F.O.B., Shenzhen). Smaller stencils are lower cost but may be difficult to support with the SMT assembly house so be sure to confirm.

The design looks fine otherwise but it is late so double check and off to the races :)
Looks great ! Keep up the great work ! Interesting that we were talking about remotes earlier today. Not sure if it has been done but consider interfacing the Logitech Harmony remote to work with the Android based XBMC sticks. Really have not searched the net on this topic but perhaps there is a possible commercial use of your work there ?
User avatar
AtomSoft
XCore Addict
Posts: 135
Joined: Mon Dec 14, 2009 3:02 pm

Postby AtomSoft » Wed Jan 29, 2014 3:24 pm

That Uart idea sounds nice. I even forgot that the XTAG has that. Thanks Ill add 1 pin to each side for it to even it out.

The pin headers i planned to use are the generic type. My first batch of these will be 3 boards and i dont want the price to be high. The goal is for it to be affordable and using parts like that while nice will raise the cost. I cannot source things like that. Im not rich enough to buy in bulk :)

The SCH isnt complete. I will rename all the GPIO NET labels so its readable today.

I plan on assembling these by hand but getting the PCBs made by OSHPark. I have a reflow oven (home made) and all the tools needed. I get stencils made from OSHStencils. they are thin but work well for small batches (~100 pcbs).

If i had a Logitech Harmony remote and an Android based XBMC stick i would try but i do not, so cant test even if i wanted to.

Thanks for the interest and info.
User avatar
AtomSoft
XCore Addict
Posts: 135
Joined: Mon Dec 14, 2009 3:02 pm

Postby AtomSoft » Wed Jan 29, 2014 4:05 pm

New Sch and Board. Im loving all the advice and stuff. Thanks again.

Image
You do not have the required permissions to view the files attached to this post.
User avatar
AtomSoft
XCore Addict
Posts: 135
Joined: Mon Dec 14, 2009 3:02 pm

Postby AtomSoft » Wed Jan 29, 2014 4:13 pm

Forgot to add the LED (labeled X0D12) It has a cut-able solder jumper for those who need that extra pin :)
You do not have the required permissions to view the files attached to this post.
User avatar
mon2
XCore Legend
Posts: 1679
Joined: Thu Jun 10, 2010 11:43 am

Postby mon2 » Wed Jan 29, 2014 5:43 pm

Looks great from this side ! OSHPark sounds interesting on how they lower their costs. If the fab they use is in China (most likely the case) then you will have a small delay due to the Chinese New Year holiday till late next week. Have fun and keep us all posted on your progress !

Who is online

Users browsing this forum: No registered users and 0 guests