| T O P I C R E V I E W |
| al1234 |
Posted - 25 Aug 2010 : 10:50:48
I was tidying a design by making connector references sequential and functionally logical on my schematic but when I “forwarded design changes” most connections were unrouted and a second “forward design changes” was required to correctly connect the now unrouted components. I’ve seen this on the forum before but the search has failed me.
This can be easily replicated by:
-
Make a new project
-
connect three resistors in series on the schematic (R1, R2, R3)
-
forward to PCB and route
-
rename R1 to R4, R2 to R1 and R4 to R2 on schematic (i.e swap idents R1 and R2)
-
forward design changes (arghh!)
-
forward design changes again (arghh! x 2)
To me this looks like a fundamental error with your underlying database. Each entity in your database should be uniquely referenced by an index that doesn’t change (a GUID?). It looks like you are referencing by component ID so swap the ID, the entities swap and I lose a day’s work. |
| 18 L A T E S T R E P L I E S (Newest First) |
| Peter Johnson |
Posted - 11 Jul 2011 : 18:32:41
Regarding the comments on 'Apply Layout Pattern'. There seems to be a Windows timing error that causes a crash on some machines when you copy directly from one design to another.
If you copy the design to the clipboard, then apply the pattern from the clipboard, this timing error is avoided and the function becomes very reliable. So the moral is, always use the clipboard as a temporary store. |
| al1234 |
Posted - 03 Jul 2011 : 21:48:19
This problem has been around fo a year.
It is reasonable to want to change refs on the schematic and to retain roiuting. Is this fixed for the new version?
(Peter - I don't like the look of your workaround it's too dangerous! so I have never used it) |
| shadders |
Posted - 24 Feb 2011 : 01:30:58
Hi Iain,
Thanks - sounds like a good idea - hard disk space is so cheap now - so not a problem. Thanks.
Regards,
Richard. |
| Iain Wilkie |
Posted - 23 Feb 2011 : 17:49:40
I have mine set to back up every 10 minutes and 10 levels of backup .... this allows me to go back 100 minutes.
Iain
|
| shadders |
Posted - 23 Feb 2011 : 14:25:34
Hi Iain,
Thanks - i will look into that feature - i did examine the "tilde" security save - but this had been overwritten.
Thanks and regards,
Richard. |
| Iain Wilkie |
Posted - 23 Feb 2011 : 08:16:38
Remember you can set EasyPC up so that it automatically creates any number of backups at a given interval ..... so even if you are not backing up manually, there are back-ups in the background that you can always go back to .... used this many times !
Iain
|
| shadders |
Posted - 23 Feb 2011 : 01:45:12
Hi,
Thanks for the feedback and guidance.
I think i will stick with the easy option - do not place components etc, until all have been renumbered.
Or renumber in PCB and back annotate.
I did save at regular intervals in first iteration with different versions - but got lazy this time.
Thanks again for all the help.
Regards,
Richard. |
| KevL |
Posted - 22 Feb 2011 : 17:24:43
Peter
I haven't tried this method you describe but last time I used the apply layout pattern I found it extremely susceptible to crashing horribly. Has this been improved recently?
I raise the point in the constructive hope of avoiding users loosing work etc. Backup all designs before forwarding design changes involving renumbering and maybe before applying layout patterns. Better safe than sorry.
K |
| Peter Johnson |
Posted - 22 Feb 2011 : 10:12:04
This isn't an excuse for not doing work, but there's a way to avoid this, providing you have a copy of the pcb before the changes were forwarded.
Temporarily group the whole of the schematic with a group which is carried forward to the pcb.
Forward changes (Aaargh! time)
Open your backup pcb, select all, and copy to clipboard with <Ctrl+C>
Go to unrouted current pcb. Select [Tools], [Apply Layout Pattern], and copy from clipboard to the group name for the whols pcb. Voila! The rerouted pcb is now floating under the cursor ready for placement.
Please check the result against the backup in case it's got some details wrong - it's a complex function, so there is room for errors. |
| shadders |
Posted - 14 Feb 2011 : 09:27:47
Hi Iain,
Thanks.
I auto-renumbered in schematic and this is what caused the problem. Only after a few saves did i then forward design changes - and i did not save different versions as i was going - so i lost quite a bit of placement work. Anyway - it is only a hobby.
Regards,
Richard. |
| Iain Wilkie |
Posted - 14 Feb 2011 : 09:08:41
As far as I am aware (and have done many times) is that you auto re-number in the pcb editor and then back-annotate.
I have never had any issues using this method.
Iain
|
| shadders |
Posted - 13 Feb 2011 : 23:06:38
Hi ,
Not sure if this is the same problem - i thought it would be a good idea to auto renumber all components - so instead of gaps in C1 to C255, it produced a continuous list.
I did not realise that if you do not forward design changes, that you can continue to edit in PCB - then update the system with forward design changes later - and all components due to their new number, are now not the correct placed part on the PCB, and all routing has been removed showing everything as yellow rubber bands.
Is this how it is meant to work ?.
I would have thought that if i used this feature, that all components already placed in PCB would have been given a new number, and this would correlate with the schematic number.
Regards,
Richard. |
| KevL |
Posted - 27 Aug 2010 : 14:57:31
I too would really like to have this fixed urgently. The cause is obvious and the fix (the two pass renaming scheme) is trivial to implement.
K
|
| pedro444 |
Posted - 27 Aug 2010 : 14:45:43
I've got into the habit of taking a complete copy of the folder containing the design prior to any renames or re-annotates.
Then if/when it all falls apart I just overwrite everything with the copy. It doesn't fix the problem but it does save fumbling around with the backups. |
| al1234 |
Posted - 26 Aug 2010 : 14:33:46
Hi David / Peter,
Could we have a response / way forward for this problem. It's been around for too long, in many posts and has been ignored by several major updates.
As I described earlier a schematic design in which components are internally linked in the database to the PCB components by their component reference (a variable) is a recipe for disaster!
Thanks
Al |
| KevL |
Posted - 25 Aug 2010 : 12:28:40
This has been reported in the past. The problem is that the renaming algorithm is weak (buggy????). If it makes the changes you describe then half way through the renaming process then there will be duplicate reference designators. It cant allow this so rips the board up (effectively). Fix would be for the software to rename all - to be renamed parts - to say $$$R1, $$$R2 etc as first pass. Then rename $$$R1 to R4 as needed. Renaming takes a little longer but only by a few milliseconds. Much better than hours of wasted work.
Kev |
| al1234 |
Posted - 25 Aug 2010 : 11:35:08
Thanks Iain,
That's the workaround.
But both methods should work and it's a clue to a fundamental problem that'll only come back and bite.
Anyway - back to re-routing my design. I turned off my McAfee auto-backup because it's not compatible with EasyPC. (see previous post) so back to manual backup...
Al |
| Iain Wilkie |
Posted - 25 Aug 2010 : 11:25:06
Renaming of components should be done in the PCB editor and then back annotated. Then all will be well.
Iain |
