Hidden designators or comments on PCB layout - Protel 99SE

Rob, there are several possibilities and it sounds like you have a good idea what they could be but haven't had any luck yet.

For a comment (I assume that you are not displaying them) use the global edit function combined with the position ("center") to bring them all to the center of the components. Possibly make all comments visible with a global edit first.

A designator could be done similarly but then you have to re-arrange all your other designators afterward. Not so good but if you have to, you have to. Also make sure that all designators are visible with a global edit.

Another common one outside the board area is a polygon that was moved without knowing it, like when it was not deselected and you moved something else. This is doubly troubling when the polygon may have the remove dead copper turned on. If it is outside a valid net connection then the whole polygon disappears after pouring.

Is there any possibility it is a component primitive? Did you ever unlock component "primitives" (not the lock component)? That can be tough as well because you may not know which component it may belong to.

There are various selection problems with items outside your board or in the negative quadrant areas. Not all selection methods work, one that worked with one item may not work with another item.

You seem to have tried using the select outside area, I have typically not found it to work with your type of problem. Try this, use select all (S,A) move the board and all other items in a direction that should bring the errant item into view. Watch the bounding box around your selection as you move it to give you hints on which direction and how much to move. If you bring the item into positive quadrant space then you can easily deal with it.

If the previous methods don't prove useful try, select all (S,A), the use deselect inside (E, E, I) and draw a bounding box around your proper board area, be generous allow an inch or two at least around your board or other desired items. Once the proper board area is deselected then delete selected (Shift and Delete).

Hopefully one of those works. As a last resort you could try saving the file in ASCII format and edit it with some text editor to try and find the offending object. Edit it's coordinates to bring back to the positive quadrant at a known location.

--
Sincerely,
Brad Velander


"Rob"  wrote in message
news:41a023f2$0$25760$5a62ac22@per-qv1-newsreader-01.iinet.net.au...
> I\'ve laid out a board and have what I suspect is a hidden
comment or
> designator way outside the board layout. Clicking view all
displays the PCB
> in a small portion of the screen instead of filling the full
field of view.
> I\'ve tried unhiding all and looking for whatever it is outside
the board
> area and also selecting all outside the board area (and then
deleting
> deletion) without any luck.
>
> Any suggestions as to the problem. Thanks
> rob
>
>
Reply to
Brad Velander
Loading thread data ...

By default, Protel 99SE creates "rooms" on th PCB for each schematic - for a multi-sheet schematic, these rooms are laid out marching off to the top right, and the room outline layer is turned off. This results in a "zoom all" squeezing the PCB down to the bottom left, to leave room for the hidden rooms.

There are a couple of check boxes at the bottom of the "Update PCB" form that are checked by default - uncheck these to prevent rooms from being generated, and delete the rooms in PCB.

--
Peter Bennett, VE7CEI  
peterbb4 (at) interchange.ubc.ca  
new newsgroup users info : http://vancouver-webpages.com/nnq
GPS and NMEA info: http://vancouver-webpages.com/peter
Vancouver Power Squadron: http://vancouver.powersquadron.ca
Reply to
Peter Bennett

I've laid out a board and have what I suspect is a hidden comment or designator way outside the board layout. Clicking view all displays the PCB in a small portion of the screen instead of filling the full field of view. I've tried unhiding all and looking for whatever it is outside the board area and also selecting all outside the board area (and then deleting deletion) without any luck.

Any suggestions as to the problem. Thanks rob

Reply to
Rob

Many thanks for the reply & suggestions Brad (& Simon).

I ended up selecting the board area and pasting it into a new pcb document. Whatever was causing the problem was left behind. My bet it was a poly that was dragged off to the side when it was inadvertently selected. Either way I learnt something new - your suggestion for centring the comments etc will probably save me next time!

thanks rob

Reply to
Rob

If its a designator or comment and in the negative space.. what your suggesting has no effect. The best method is to select all and move the entire design to say 10000 10000 (10 inches) from the zero zero reference point. Then you should be able to see anything outside the area. You will, of course, note that when you move everything, their is a box placed around where Protel thinks its extent is.. take a good note.. one edge will have the problem!

Simon

PCB

view.

Reply to
Simon Peacock

ElectronDepot website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.