DXP and dulplicate components
Bookmark this page:
 Yahoo!
 Google
 Windows Live
 del.icio.us
 digg
 Netscape
|
|
||||||||||||||||||||||
|
Posted by JamesB on April 30, 2008, 9:41 am
Please log in for more thread options I've got a problem with DXP. When viewing the gerbers, it appears that we have some components duplicated outside of the board area, but only on certain layers - specifically the solder and paste layers, but not on the normal top layer. I've tried the old trick of selecting outside area and trying to delete them but they won't show up at all in Protel. Using the inspector list, I can't see them either and definately can't delete them. Any ideas? Thanks, -- James | ||||||||||||||||||||||
|
Posted by TT_Man on April 30, 2008, 10:28 am
Please log in for more thread options Typical..... how about turning all layers on and retrying? I've found library errors that cause similar problems in the old 'Client' version and the culprit was in an odd ball layer. | ||||||||||||||||||||||
|
Posted by Brad Velander on May 1, 2008, 2:03 am
Please log in for more thread options My suggestion,
Check all your library parts used in the design in the library editor, check that none of them have extraneous bits spread out away from the main body of the part. In the library viewer window the part should roughly come in filling the screen (either X or Y) with all layers turned on so you can see anything on any layer. If it comes in smaller, then there is probably a primitive spread out away from the main body of the part. Then update the PCB parts from the library once you have confirmed your library parts are alright. I suspect that you have gotten some primitives from a land pattern/footprint accidently moved out to the extremes of the database. If you get it fixed, make sure that all your land patterns have their primitives locked so that they cannot be moved separate from the whole land pattern again. That's my best guess at what may be going on. To try and just remove the problem, the selection trick that should work is actually. Turn on all used layers. Select All, then Deselect Inside mousing just around your board outline, then Shift-Delete. The details of this operation are: This selects everything regardless of it's location. Then you deselect anything within the board outline. Then delete the still selected items. The key operation is the Deselect anything bounded by the board outline. If it is even a segment of a land pattern that was moved outside the board outline, that item will not be deselected by bounding the board outline. Then when you Shift Delete, you will remove that offending item with remnants out in the extremes because it was not deselected by the bounding box only around the PCB outline. If this seems to work then run the Update PCB from your schematic again, it will probably add back components that you did delete fixing the problem. Finally run your DRC to see that everything is still as per the rules and connectivity. By your original comments, the only way that soldermask portions of a part land pattern can move away from the pads is when they are added into the land pattern as a separate primitive. Otherwise most of the normal soldermask detail is calculated from the pads. Since you say there are no pads in that area, then the culprit(s) must be from land patterns that have separate soldermask primitives (fills, traces, polygons on the soldermask layers) within the land pattern. Does that help you zero in on the culrpit parts? -- Sincerely, Brad Velander. >
>> Hi,
>> >> I've got a problem with DXP. >> >> When viewing the gerbers, it appears that we have some components >> duplicated outside of the board area, but only on certain layers - >> specifically the solder and paste layers, but not on the normal top >> layer. >> >> I've tried the old trick of selecting outside area and trying to delete >> them but they won't show up at all in Protel. Using the inspector list, I >> can't see them either and definately can't delete them. >> >> Any ideas? >> >> Thanks, >> >> -- >> James | ||||||||||||||||||||||
|
Posted by JamesB on May 1, 2008, 4:20 am
Please log in for more thread options Brad Velander wrote:
[cut..] > To try and just remove the problem, the selection trick that should work
> is actually. Turn on all used layers. Select All, then Deselect Inside > mousing just around your board outline, then Shift-Delete. The details of > this operation are: This selects everything regardless of it's location. > Then you deselect anything within the board outline. Then delete the still > selected items. > The key operation is the Deselect anything bounded by the board outline. > If it is even a segment of a land pattern that was moved outside the board > outline, that item will not be deselected by bounding the board outline. > Then when you Shift Delete, you will remove that offending item with > remnants out in the extremes because it was not deselected by the bounding > box only around the PCB outline. If this seems to work then run the Update > PCB from your schematic again, it will probably add back components that you > did delete fixing the problem. Finally run your DRC to see that everything > is still as per the rules and connectivity. > > By your original comments, the only way that soldermask portions of a > part land pattern can move away from the pads is when they are added into > the land pattern as a separate primitive. Otherwise most of the normal > soldermask detail is calculated from the pads. Since you say there are no > pads in that area, then the culprit(s) must be from land patterns that have > separate soldermask primitives (fills, traces, polygons on the soldermask > layers) within the land pattern. Does that help you zero in on the culrpit > parts? Thanks Brad. I did your select trick which solvevd the problem. Funnily enough, re-updating the PCB didn't cause any changes and the problem hasn't come back. Love to know why that happened, but I've given up trying to find logic with DXP sometimes. Thanks, -- James | ||||||||||||||||||||||
|
Posted by TT_Man on May 1, 2008, 4:47 am
Please log in for more thread options
>
> Thanks Brad. I did your select trick which solvevd the problem. Funnily > enough, re-updating the PCB didn't cause any changes and the problem > hasn't come back. > > Love to know why that happened, but I've given up trying to find logic > with DXP sometimes. > > Thanks, > > -- > James You and half the other protel users around the world no doubt.... A similar thing happens with copy .sch to new.sch and part of the .sch is outside the paper size box..... Rather the devil you know, I suppose. | ||||||||||||||||||||||
>
> I've got a problem with DXP.
>
> When viewing the gerbers, it appears that we have some components
> duplicated outside of the board area, but only on certain layers -
> specifically the solder and paste layers, but not on the normal top layer.
>
> I've tried the old trick of selecting outside area and trying to delete
> them but they won't show up at all in Protel. Using the inspector list, I
> can't see them either and definately can't delete them.
>
> Any ideas?
>
> Thanks,
>
> --
> James