On 12:25 PM 13/08/2001 +0200, [EMAIL PROTECTED] said:
>Hello all,
>I dont know what I have done to get this warning, but it keeps me bothering.
>I never had the intention to place any prims on the internal plane. Does
>anyone know how this can happen, or better how to find this prim. to delete

A few things could be happening here:

1) the simplest - there is some text or line or fill or something that has 
been placed/moved the internal plane.  In this case you can get rid of it 
(assuming you want to) by turning the internal layer on, change to the 
internal plane and then use S-Y  (Select all on laYer).  This should 
highlight any free entities on the layer.  Before you delete anything make 
sure that you have not got extra bits selected (use X-A before the 
S-Y).  One way of identifying what is causing the problem if it is not 
clear from the selection is to copy and past the selection into a new blank 
PCB and then zoom all should show what the primitive is, at least, and this 
may help you track it down.  You can also use M-S (Move-Selection) to try 
to gauge how big the object is by seeing how big the move selection 
rectangle is.  If the object is smaller than the selection box then you 
should find that the cursor is hugging the opposite corner of the move 
selection box.  This can help narrow the search.

It is common to have tracks around the outside of the PCB on the internal 
layers to pull back the plane from the edge of the board.  So all my 
release boards that have internal planes will get this warning.  In fact I 
know I have forgotten something if I do not get it.

Layer clocks or stack-up indicators will usually have fills and text on the 
internal layers.  These will cause the warning to appear.

*But* since it is also possible that the entities that are on the internal 
layer are not free entities and so 1) will not work...most of what remains 
assumes that the offending primitive is small and so easily missed. If the 
offending primitive(s) are large then they will show up by simply turning 
on all the internal plane layers.

2) Painful and care required - make all the other layer colours dim or turn 
them off but each internal layer a bright bold colour.  Then scan carefully 
looking for something standing out.  This is not always reliable when the 
offending primitive is small. (I have never had a case where I was tracking 
down a small primitive on an internal plane - this is a technique I use in 
other situations.)

3) Produce gerbers for the board and check to see if anything strange 
appears - other than automatic blowouts and reliefs.

4) Do the same with a printout.

5) Check library components for embedded primitives on the internal layer.

6) Save the PCB file as an ASCII file and then open it in a text editor and 
search for anything on the any internal layers.  It may help to 
deliberately add a known track on one or more internal layers so you can 
determine the format of the layer specification and you know if your search 
is working correctly.  This method should be pretty reliable in finding the 
objects.  Interpreting the information so you can determine what component, 
or union or polygon or whatever is a little more complex but with some 
thought and a bit of study of the ASCII format it can be done.  If things 
are getting tough this is my "big hammer".

There are probably other things as well.  Have you got any more info.

Ian Wilson

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*                      - or email -
* mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum
* Contact the list manager:
* Browse or Search previous postings:
* http://www.mail-archive.com/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to