Ian,
   For some reason when I originally went to put a pad on the top solder 
layer, I could not find it! I am not sure what I had done, but my best 
guess is that I was trying to place a via rather than a pad.
    Thanks for getting me to recheck this, as I do not like to use the 
update primitives unless I "really" have to.

   The only disadvantage I see is that you must specify the solder mask 
pad size to include the expansion around the BGA pad in the component 
library, rather than allowing it to be specified in the board rules (I 
am not real sure if a rule can be set up to allow expansion for a pad 
that exists on the TopSolder layer. I tried it and it did not appear to 
work, but I need to investigate further.)

David


Ian Wilson wrote:

> On 01:12 PM 1/06/2002 -0500, David W. Gulley said:
> 
>> Richard Sumner wrote:
>>
>>> David,
>>> Talk to your assembler before you invest time in this. The paste mask 
>>> becomes a metal stencil for applying the solder paste. So donuts will 
>>> not work (the donut hole is unsupported).
>>
>>
>>
>> Actually my idea was to make the width of the track greater than 2x 
>> the radius of the arc so I would end up with a "filled donut". (For 
>> example if I want a 30 mil opening in the paste mask, I could use a 
>> 20mil wide arc with a radius of 5mil.)
>>
>> However, what I have just tried that seems a bit simpler is to use a 
>> pad and a via (gee a via in a pad!) where the pad is TopLayer only and 
>> the via is set for tenting. Do an update free primitives after import 
>> to the PCB and viola...
> 
> 
> 
> Alternatively, you can use thru-hole pads fully tented (see the advanced 
> tab of the pad properties) and add another single layer 0mm hole size 
> pad on just the *top mask* layer.  Make sure you don't tag this one as 
> tented - a tented mask pad makes for nothing (a small improvement in 
> P99SE would be that single layer pads on the mask layers can't be 
> tented).  This works OK.  So you fully tent and then open the mask 
> manually in a controlled fashion.  P99SE allows pads to exist on 
> non-copper layers - a great thing I think.
> 
> This way may have a small advantage over your method as it does not 
> require two copper primitives - that then have to be updated to force 
> the pads nets onto the accompanying vias.
> 
> You may need to muck about with the paste layer as well to close it off 
> as required - but you have this issue regardless.
> 
> Ian Wilson
> 
> ____________________________________________________________
> Considered Solutions Pty Ltd     mailto:[EMAIL PROTECTED]
> ABN: 96 088 410 002
> 5 The Crescent
> CHATSWOOD   2067
> Ph: +61 2 9411 4248   Fax: +61 2 9411 4249
> 



-- 
David W. Gulley
Destiny Designs


* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Forum Guidelines Rules:
* http://www.techservinc.com/protelusers/forumrules.html
*
* Browse or Search previous postings:
* http://www.mail-archive.com/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to