On 09:25 AM 14/03/2002 +0000, [EMAIL PROTECTED] said:
>Quoting Brad Velander <[EMAIL PROTECTED]>:
> > Kiernan,
> >       Ian's explanation below is correct. What you're seeing are drawn
> > pads rather then flashed rectangular pads. A major shortcoming of Protel
> > if
> > you are doing very fine or finicky work. As for your soldermask
> > encroachment, that will not be an issue because the soldermask pad will
> > be
> > drawn similarly and won't encroach.
>Thanks guys. We're using FPC connectors with an 0.3mm pitch. I've got the 
>designed so that there's virtually no visible land after soldering, so I will
>get soldermask encroachment under the pad even though the soldermask lines up
>with the copper because the pad that I'm getting out of the gerber is smaller
>than the one on the screen (ie smaller than the pin). At the very least, I'll
>get severe solderballing.
>I've put a sample of the gerber output for a couple of pads below and I 
>whether anyone knows enough about gerber to see if there's a quick fix that
>will produce the correct result. One of the pads is supposed to be a 
>and the other actually uses the octagonal option.
>Are there any other Non-WYSIWYG features that I should know about before I
>spend too many hours on this?? I thought gerber output was the gold standard
>for PCB packages.
>Kiernan Fitzpatrick


Small rectangular pads should be flashed, if they are 0, 90 180 or 270 
degrees, as others have mentioned.  So we will assume that your radial 
board requires off-angle pads.  If not then there is something odd going on.

We have traditionally just removed the soldermask in a strip from narrow 
pitch SM details such as connectors and fine line devices so the mask 
encroachment is a non-issue for us.  We have not had any problems with 
bridging or balling.

You may be able to get the off-angle pads to be drawn with a smaller 
aperture by making sure there is a very fine feature in the design (so draw 
a thin track on an unused mech layer with a 2 thou track or even less).  If 
you do this you may want to change you Gerber resolution away from the 
default three decimal figures to 4 to ensure good plotting accuracy.  If 
you can get a smaller radius corner you problem will largely disappear 
won't it? Especially if you pull the mask away a little more.

Also you can try to tighten up the aperture matching in the CAM output, 
which may help.

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