See point 2 in the following kb item.
Gyula Hegyesi

Protel Knowledge Base

Item - 1694

Logged: 3/30/1998 Revised:7/30/2001 Item categories: Autorouting Products affected: Protel 98 (All Versions);99 (All Versions); Operating systems affected: Windows 95;98;NT;
Query: Why won't my board autoroute?
Details: Sometimes when attempting to route a PCB file in
Advanced Route, it can remain in the Initializing shape based
route pass, or stop after Initializing.
Answer: Use the following points to help identify why the board
will not route;

1. Check that the PCB outline has been placed on the Keep Out
Layer and not a Mechanical Layer. (For example, make sure
that the Keep Out Layer is used instead of Mechanical Layer 1
as these 2 layers are the same color).

2. Insure that there is some outline on the Keep Out Layer. It has
been found that the outline need not be completely closed, i.e.
the corners do not need to touch. Arcs are not supported in
board outline on the Keepout Layer. They are ignored. This is
the reason why a board outline defined by a full arc will not
initialize and start routing. In the case where tracks and arcs make up the board outline,
the arcs get ignored and in effect a straight line is used to close
up the gap of where the arc was placed. Generally, in place of
the arc there is a straight line assumed from and to the nearby
tracks on the Keep out layer.

3. Enable all the layers that are needed for routing the PCB in
the Design Rule Routing Layers setup. When setting up the
routing layers you will need to keep in mind that the present
autorouter requires either the top or bottom layer to be enabled
in the Routing Layers setup.
Otherwise you will receive the error message "Design Rule
Error: no pads defined on any layers". Pressing OK will close
down this error and it will appear to want to start autorouting by
prompting you to change the routing grid to 0mil. The end result
is that the autorouter will be unable to initialize.

4. Avoid using net names with hyphens, spaces; characters
other than the alphabet and numbers.

5. Maintain net names less than 10 characters.

6. Maintain pad designator names to 4 characters or less.

7. In Route 98, the router requires all parts of the board to be
within a 32x32 inch region from the absolute workspace origin
(not the set-able current origin). Note that the coordinates on the
Status bar display the distance from the set-able current origin,
so if you are not sure reset the origin. To reset the origin select
Edit Origin Reset from the menus. In Route 99, the autorouter workspace is the same as the PCB
workspace of 100x100 inch.

8. Avoid placing any polygons prior to routing. This includes
split planes.

9. Polygons that are placed on the top or bottom overlay, or
mechanical layers can prevent the autorouter from initializing
and routing the PCB. This includes polygons that have been
included in a footprint. You will need to edit the footprint and
remove the polygon.

10. Check for polygons that are not visible. See Item 2434 for
more details.

11. Avoid placing components on a grid smaller than 1mil. It is
recommended that components be aligned to a 5mil grid. On
high density PCBs, too many components, tracks and other
primitives placed on fractional grids (that is less than 1mil grid)
can cause the autorouter to find too many contentions. A
message similar to "One or too many contentions have been
found.." The only remedy to this situation is to place
components and any routed tracks on at least 1mil grid.

12. Avoid placing tracks, arcs, etc on the multilayer. The router
fails to start when it finds primitives other than pads/vias on the
multilayer within the keepout region. If you move these
primitives temporarily outside the keepout region the autorouter
will start to route the PCB.

13. Check the PCB against the maximum capabilities of the
autorouter listed in Item 2214. This includes the number of
components, pins, etc.

Brad Velander wrote:
        I don't use the autorouter at all but I have to ask about your
multilayer lines. Were any segments of these lines actually arcs? Like at
the ends of your slot? The Protel autorouter does not like arcs, I don't
know the exact connotation of that statement but on numerous occasions the
comment has been raised by those that do use the autorouter. Commonly it is
in regards to the board outline (possibly that's on the keepout layer).

Brad Velander,
Lead PCB Designer,
Norsat International Inc.,
#300 - 4401 Still Creek Dr.,
Burnaby, B.C., V5C 6G9.
Tel. (604) 292-9089 direct
Fax (604) 292-9010

> -----Original Message-----
> From: G. Allbee [mailto:[EMAIL PROTECTED]]
> Sent: Tuesday, September 11, 2001 7:47 PM
> To: Protel EDA Forum
> Subject: Re: [PEDA] Autorouting Problems
> I worked on it all day and finally found the problem.(1 day late on
> delivery)
> In this revision of the board I added a slot in the middle of
> the board.  I
> remembered an email from this group some time ago that said
> something like
> put a through hole on each end of the slot and then draw lines on the
> perimeter of the slot.  So this is what I did, however I used lines on
> multilayer figuring they would also work as keepouts and
> prevent routing in
> the slot.
> I discovered that the multilayer lines were preventing the
> autorouter from
> routing and when changed to a mechanical layer the router
> would work like
> normal..  Hmmm - a bug?
> Regards,
> Gary Allbee

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
* To leave this list visit:
* Contact the list manager:
* Forum Guidelines Rules:
* Browse or Search previous postings:
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to