Hello All,

as promised, i will inform you about the progress with our polygon pouring
problem.

I have send our database-file to the Altium Switzerland support center.
They have checked the file and have given us the following statement:

"I've looked at the polygon board, the problem was related to the teardrops.
Removing them, or changing them from arcs to tracks solved the problem..."
"This issue will be fixed in the next release."

So it is a bug!
(And i hope, it will really be fixed in the next relaese.)


Florian


> -----Ursprungliche Nachricht-----
> Von: Florian Finsterbusch [mailto:[EMAIL PROTECTED]]
> Gesendet: Donnerstag, 6. September 2001 10:40
> An: Protel EDA Forum
> Betreff: [PEDA] AW: Problems when pouring polygons
>
>
> Hello Abd ul-Rahman,
>
> thank you for your attempts to solve the mystery of pouring polgons!
>
> I have made same tests you have suggested (see below).
>
>
> Florian
>
>
> > -----Ursprungliche Nachricht-----
> > Von: Abd ul-Rahman Lomax [mailto:[EMAIL PROTECTED]]
> > Gesendet: Donnerstag, 6. September 2001 00:05
> > An: Protel EDA Forum
> > Betreff: Re: [PEDA] Problems when pouring polygons
> >
> >
> > At 09:56 AM 9/5/01 +0200, Florian Finsterbusch wrote:
> > >On our multilayer board the top and bottom layer should be
> > connected to GND.
> > >For that purpose we have placed polygons on both layers.
> > >The polygons are connected to the GND net.
> > >The pads should be surrounded by arcs.
> > >Grid Size = 0.2 mm, Track Width = 0.22 mm
> >
> > First of all, set the grid to zero. I also recommend using
> imperial units
> > for the track width, though I am not sure that this will make a
> > difference;
> > it's just that the Protel internal database is imperial so you
> > might get a
> > slightly better pour.
> >
>
> No cure
>
> > >When protel is pouring the polygon, we have rectangles around
> some pads.
> > >Also we have rectangular openings in the polygon itself!
> >
> > Something like this is to be expected under some conditions. For some
> > reason the pour routine is unable to place the fill tracks; if an arc is
> > missing, any opening left will be rectangular, if one has 90 degree
> > hatching selected. Mr. Finsterbusch did not state his setting for the
> > minimum primitive size. If this is too large there will likely
> be missing
> > primitives. This would only get worse with a fixed grid size.
> >
> > A minimum length of zero seems to work fine. However, under some
> > conditions
> > this could result in too many pour tracks and I would not be terribly
> > surprised if Protel crashed. I leave it at 1 mil. One could make
> > it smaller
> > than that.
> >
>
> My minimum primitive size was 3 mils.
> Changing it to 1 mil makes no difference.
>
> > Try setting hatching style to "No Hatching" and turn off "Remove Dead
> > Copper." This will show you only the pad clearance outlines and
> > the outline
> > of the polygon. With this setting, polygon pour will surround
> > each pad with
> > an arc or octagon (octagons may reduce plot size if software arcs
> > are used)
> > *if* the clearance rules will allow it. The grid size has no effect on
> > this. If you are not getting an outline around a pad, there are two
> > possibilities:
> >
>
> Some vias have got no surrounding arcs!
>
> > (1) your clearance rules will not allow it.
> > (2) there is a bug. I think I have seen some circumstances
> where the pour
> > outlines are incomplete, but it is difficult to reproduce and I
> > don't have
> > an example handy.
> >
> > Number (1) is the most likely cause. Try placing a line or arc primitive
> > where you think a missing primitive would be. Assign it the GND
> net. Does
> > this create a clearance violation? If so, no wonder the pour does not
> > complete the fill!
>
> Placing the arcs manually and assigning them to GND produces no clearance
> violation
> Because of that i am thinking it is reallay a Protel bug!
>
> >
> > Then, if hatching is turned on, fill track will be added. This
> > track is *on
> > grid*. If your grid setting does not meld well with the pad placements,
> > some fill tracks will be missing, causing rectangular holes in
> your pour.
> > For this reason, set the grid to zero. Protel properly
> interprets this as
> > meaning "fill gridless." This is generally recommended, it should be the
> > default setting!
> >
> > There is little reason to use cross-hatching (90 degrees or 45 degrees)
> > when grid is set to zero and a very small primitive length is
> > used. It will
> > just add extra lines. Note, however, that lines which are
> > precisely butted
> > up next to each other can display a very fine gap, either in PCB
> > or in some
> > gerber viewers. That is not real, it is a display artifact. But
> if one is
> > not willing to tolerate the appearance of this false gap -- it
> should not
> > be on the film -- then using cross-hatching will eliminate it.
> > That may be
> > a better solution than using a pour grid and a slightly oversize track.
> >
> > There are other possible causes for missing track. For example,
> > there might
> > be a layer-specific keepout primitive that is invisible, or some
> > other rule
> > interaction. Note that there are design rule clearance settings for
> > polygons which are in addition to the other clearance rules. (Most
> > designers would prefer larger clearances on polygons than elsewhere on a
> > layer because the polygon clearances are everywhere and thus more
> > likely to
> > cause fabrication or soldering problems.)
> >
> > If the cause of the problem is not found, I recommend creating a
> > small file
> > that shows the problem. (Edit down your existing file). This will help
> > Protel, but before sending it to Protel, submit it to me or to
> > another user
> > who has indicated a willingness to look at it -- don't attempt
> to send it
> > to the list!)
> >
> > If there turns out to be a bug here, we can then add this to the
> > bug database.
> >
> > [EMAIL PROTECTED]
> > Abdulrahman Lomax
> > Easthampton, Massachusetts USA
> >
>

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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