Here is a possible manual way of handling this problem,

1. tent all vias on the pcb.

2. select and copy all the vias that you would like to have tented only on
one side. unselect the currently selected vias.

3. Now paste the copied vias back onto their original location and while
still selected use the "convert selected vias to free pads" command to
change all of the newly pasted vias to free pads. You may at this point want
to give a special name to all these selected pads (ie "nt" for no tent). you
will also need to change the layer of these selected pads to the appropriate
solder mask layer and set the hole size to 0mil and expand the X and Y
dimensions by 2 or 4 mils to provide for solder mask expansion requirements.

This is manual but an quick and easy fix.

Daniel Webster

-----Original Message-----
From: Ian Wilson [mailto:[EMAIL PROTECTED]]
Sent: Thursday, September 19, 2002 1:36 AM
To: Protel EDA Forum
Subject: Re: [PEDA] Selective tenting on one side only

On 08:21 AM 19/09/2002 +0200, Kulajew Waldemar said:

>IMHO the problem is the design rules are mighty, but not mighty enough to 
>handle a rule like:
>DesignRule|Manufactoring|SolderMaskExpansion -> scope [Via AND TopSolder]

The P99SE DRC system does not consider multi-layer entities as also 
existing on the various copper layers.  This is why Kulajew's rule does not 
work.  I have raised this with Altium on a number of occasions.  It is a 
structural issue I gather.  It is not a bug but a limitation of the 
underlying architecture.  To us users, though, it is annoying.

Selective tenting was not considered a major issue (if it was considered at 
all) when P99SE was developed, and the underlying concept that multi-layer 
objects are not part of the individual copper layers from the rules POV 
possibly predates that some time as well.

I have not checked whether DXP is clever enough to know that a multilayer 
pad also exists on each copper layer but it does support selective tenting.

Ian Wilson

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
* Contact the list manager:
* 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