| |
| 30 Apr 2008 14:41:42 |
| JamesB |
| DXP and dulplicate components |
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 |
| 30 Apr 2008 14:28:28 |
| TT_Man |
| Re: DXP and dulplicate components |
"JamesB" <usenet@mesb.co.uk > wrote in message news:fv9sv4$qoc$1@aioe.org... > 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 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. |
| 01 May 2008 06:03:47 |
| Brad Velander |
| Re: DXP and dulplicate components |
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. "TT_Man" <Someone@ntlworld.com > wrote in message news:gm%Rj.60714$h65.42081@newsfe2-gui.ntli.net... > > "JamesB" <usenet@mesb.co.uk> wrote in message > news:fv9sv4$qoc$1@aioe.org... >> 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 |
| 01 May 2008 09:20:15 |
| JamesB |
| Re: DXP and dulplicate components |
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 |
| 01 May 2008 08:47:58 |
| TT_Man |
| Re: DXP and dulplicate components |
> > 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. |
| 01 May 2008 11:03:24 |
| Anton Erasmus |
| Re: DXP and dulplicate components |
On Wed, 30 Apr 2008 14:28:28 GMT, "TT_Man" <Someone@ntlworld.com > wrote: > >"JamesB" <usenet@mesb.co.uk> wrote in message news:fv9sv4$qoc$1@aioe.org... >> 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 > >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. > I have seen this sort of thing as well. Sometimes it is a very small section of arc which has a big radius with the centre outside the visible area. These arcs cannot be selected and deleted. I have exported such files in ASCII format, and deleted the relevant ARC's in a text editor. Regards Anton Erasmus |
| 02 May 2008 05:55:06 |
| Brad Velander |
| Re: DXP and dulplicate components |
James, Glad I could help. That selection/delete technique is almost fool proof. Other combinations or variations may work in limited cases but the one that I explained is the most common one to fix these problems because everything is selected, then the desired and well behaved section of the selection is removed from the selection and the unruly bits are deleted. But there are some very unique cases where it doesn't work either. That selection and deletion routine also works with the infamous items in the unviewable negative quadrants of the database, i.e. less than zero on either the X or Y axis. How you got there? Well the most common manner in which someone gets to that point is via the fact that they copied-pasted or moved something while they inadvertently had something else selected, somewhere outside of their current view/section o fthe design. When they move what they want to move they also copy/duplicate/move something that they were unaware they had selected at the time and it ends up somewhere out in the boonies. The most important practice to force into your brain is to "X" (Deselect), "A"ll before making a selection(s) for any copy or move operations. The items that you deleted must not have been anything important to the design if a subsequent update from the schematic did not add anything back in. I had suspected that maybe the operation would remove a spread out footprint and then the update would bring in a fresh one. AD/DXP/Protel is actually a fairly logical package, however too many people compare it against their former tools in determining their view of that logic and a lot of the other tools are not that logical when examined with pure logic in mind. I have used a number of them over my years and they all have their quirks to one extent or the other. The largest number of complaints definitely come from users forced to switch over but that is always the case with every package. Most are being forced to change from another package, not changing by choice. After a while a number of them do eventually see that light and only look for improvements, not to turn the whole package upside down. -- Sincerely, Brad Velander. "JamesB" <usenet@mesb.co.uk > wrote in message news:fvbufp$g2c$1@aioe.org... > > 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 |