Forums

PCB layout for LPC2294

Started by itsashish_iitk June 24, 2006
Hi,

I am designing the pcb for a wireless sesor network using cypress IC. I
am using LPC2294 controller for the same. I have made the schematic and
done the component placement in pcb designing. But during the routing I
am facing the problem as the pins in the LPC2294 controller are close.
I am using the protell99SE for pcb designing. The design rules I choose
as the 10mil track width and 10mil spacing between the track. I am
using autorouting feature of the software.

Somebody please help me in choosing the proper design rules and any
other tips which helps me in competing the design.

TIA

Ashish

An Engineer's Guide to the LPC2100 Series

Hi Ashish,

Can you measure the distance between edges of the pins ?

In the datasheet the package outline says, distance between centre of pins is 0.5 mm (19.6 mil) and each pin is 0.27 mm max (10.6 mil). Which means clearance between pins is 19.6 -10.6=9 mil. So if you change the clearance to 9 mil errors should not appear. Track width can be still kept at 10 mil, since indivindual pins of the controller are greater than 10 mil.

Bye,
Praval

itsashish_iitk wrote: Hi,

I am designing the pcb for a wireless sesor network using cypress IC. I
am using LPC2294 controller for the same. I have made the schematic and
done the component placement in pcb designing. But during the routing I
am facing the problem as the pins in the LPC2294 controller are close.
I am using the protell99SE for pcb designing. The design rules I choose
as the 10mil track width and 10mil spacing between the track. I am
using autorouting feature of the software.

Somebody please help me in choosing the proper design rules and any
other tips which helps me in competing the design.

TIA

Ashish






---------------------------------
Ring'em or ping'em. Make PC-to-phone calls as low as 1/min with Yahoo! Messenger with Voice.







Hi,

Change the rule to 7 mill for spacing and trace size. I am designing
with DXP 2006 and needed to change it to those rules.

regards,
Charles

--- In l..., "itsashish_iitk"
wrote:
>
> Hi,
>
> I am designing the pcb for a wireless sesor network using cypress IC. I
> am using LPC2294 controller for the same. I have made the schematic and
> done the component placement in pcb designing. But during the routing I
> am facing the problem as the pins in the LPC2294 controller are close.
> I am using the protell99SE for pcb designing. The design rules I choose
> as the 10mil track width and 10mil spacing between the track. I am
> using autorouting feature of the software.
>
> Somebody please help me in choosing the proper design rules and any
> other tips which helps me in competing the design.
>
> TIA
>
> Ashish
>

Hi,

WIll that small tack size and spacing not create any problem in fabrication and working of the design?
Please let me know if you got the board fabricated with these rules. Also please let me know whether you are using autorouting or manual routing.

Thanks
Ashish

charlesgrenz wrote: Hi,

Change the rule to 7 mill for spacing and trace size. I am designing
with DXP 2006 and needed to change it to those rules.

regards,
Charles

--- In l..., "itsashish_iitk"
wrote:
>
> Hi,
>
> I am designing the pcb for a wireless sesor network using cypress IC. I
> am using LPC2294 controller for the same. I have made the schematic and
> done the component placement in pcb designing. But during the routing I
> am facing the problem as the pins in the LPC2294 controller are close.
> I am using the protell99SE for pcb designing. The design rules I choose
> as the 10mil track width and 10mil spacing between the track. I am
> using autorouting feature of the software.
>
> Somebody please help me in choosing the proper design rules and any
> other tips which helps me in competing the design.
>
> TIA
>
> Ashish
>

---------------------------------
Yahoo! India Answers: Share what you know. Learn something new Click here
Catch all the FIFA World Cup 2006 action on Yahoo! India Click here



> WIll that small tack size and spacing not create any problem in
fabrication and working of the design?
>

7 mil trace and space are fine and are considered easy to fabricate
these days. Sometimes I change to 7 and 8 as that is on a 15 mil
pitch so I can set the grid size to 5 mils, which makes hand editing
much easier.

8 mil drill size for vias with a 25 mil ring. Inner layers require a
43 mil keepout area (all are diameters).

If its a 2 layer board you may need to go to a bigger hole, just
because some proto shops require that for quick turn. While there are
many options for fabrication, I've been very happy with PCBexpress.

brucee
Coridium Corp (not affiliated with PCBexpress)

viskr wrote:
>> WIll that small tack size and spacing not create any problem in
>
> fabrication and working of the design?
> 7 mil trace and space are fine and are considered easy to fabricate
> these days. Sometimes I change to 7 and 8 as that is on a 15 mil
> pitch so I can set the grid size to 5 mils, which makes hand editing
> much easier.
>
> 8 mil drill size for vias with a 25 mil ring. Inner layers require a
> 43 mil keepout area (all are diameters).
>
> If its a 2 layer board you may need to go to a bigger hole, just
> because some proto shops require that for quick turn. While there are
> many options for fabrication, I've been very happy with PCBexpress.
>
> brucee
> Coridium Corp (not affiliated with PCBexpress)

I'm fond of:

http://www.barebonespcb.com/

They state minimum 6mil trace/space

They run by Advanced Circuits

http://www.advancedcircuits.com/

and have a really cool design-for-manufacturing upload service
(you can check your design, and not use them for mfg if you like)

http://www.freedfm.com/

I priced around for 6-layer boards, and the places were
all very close to Advanced Circuits, so I stuck with them.

Dave

(Not associated with any of these companies either)

David Hawkins wrote:

> viskr wrote:
> >> WIll that small tack size and spacing not create any problem in
> >
> > fabrication and working of the design?
> >
> >
> > 7 mil trace and space are fine and are considered easy to fabricate
> > these days. Sometimes I change to 7 and 8 as that is on a 15 mil
> > pitch so I can set the grid size to 5 mils, which makes hand editing
> > much easier.
> >
> > 8 mil drill size for vias with a 25 mil ring. Inner layers require a
> > 43 mil keepout area (all are diameters).
> >
> > If its a 2 layer board you may need to go to a bigger hole, just
> > because some proto shops require that for quick turn. While there are
> > many options for fabrication, I've been very happy with PCBexpress.
> >
> > brucee
> > Coridium Corp (not affiliated with PCBexpress)
>
> I'm fond of:
>
> http://www.barebone spcb.com/ They state minimum 6mil trace/space
>
> They run by Advanced Circuits
>
> http://www.advanced circuits. com/ and have a really cool design-for-manufact uring upload service
> (you can check your design, and not use them for mfg if you like)
>
I use their $33 Each service, the boards are excellent quality!

Another service I've tried is: http://www.pcbnet.com/ The quality is
not quite up the Advanced Circuits standards, but the price can be
better than the $99 minimum Advanced charges.

FWIW, I have had several SMT solder paste stencils from
http://www.smtstencil.com/ Using these and a 1500W toaster oven has
allowed me to quickly, and painlessly, prototype several LPC2000 designs.
Regards,

TomW

--
Tom Walsh - WN3L - Embedded Systems Consultant
http://openhardware.net, http://cyberiansoftware.com
"Windows? No thanks, I have work to do..."
----------------

This is an interesting thread. Does anyone know of any companies that
can assemble parts onto boards in small quantites for prototype
purposes? I'm getting too old to do my own soldering on those small parts.

I know that assembly will cost a lot more than the cost of the boards,
but it's a good thing to have someone do that job for me.

Eric

Is the spacing of 7mil between vias, between thru hole pads,between smd pad and tracks, between thru hole pad and tracks is ok.
Also can anybody please tell me the vendor in india who do good and fast fabrication of pcb. Presently I am getting it done from ability components in india. Also I need the manufacture who to the soldering of pcbs in small quantity.

TIA
Ashish

Eric Engler wrote: This is an interesting thread. Does anyone know of any companies that
can assemble parts onto boards in small quantites for prototype
purposes? I'm getting too old to do my own soldering on those small parts.

I know that assembly will cost a lot more than the cost of the boards,
but it's a good thing to have someone do that job for me.

Eric

---------------------------------
Yahoo! India Answers: Share what you know. Learn something new Click here
Catch all the FIFA World Cup 2006 action on Yahoo! India Click here



----- Original Message -----
From: "Eric Engler"
To:
Sent: Monday, June 26, 2006 5:15 AM
Subject: [lpc2000] Re: PCB layout for LPC2294
> This is an interesting thread. Does anyone know of any companies that
> can assemble parts onto boards in small quantites for prototype
> purposes? I'm getting too old to do my own soldering on those small parts.
>
> I know that assembly will cost a lot more than the cost of the boards,
> but it's a good thing to have someone do that job for me.

Active-PCB in Reading, UK.

Leon