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).


> -----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
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.
> 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:
* 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