| Author |
 Topic  |
|
|
KevL
United Kingdom
78 Posts |
 Posted - 03 Jun 2011 : 13:23:53
|
Just noticed this.
If one adds a new part in a schematic e.g. R3 and then opens up a PCB which has not yet being forward annotated (so has no R3) and one then chooses to rename on the PCB so that R2->R3, R1->R2 and then back annotates then the process will be successful.
But now there are R3 (2off) on the schematic. This is unlikely to end well.
Of course I'm only renaming stuff in the PCB and back annotating because forward annotating rips up the PCB on renames - never the less there is clearly a problem here and care might be needed that the fix does not create new problems. E.g. Cant back annotate or back annotate also renames unintended parts are obvious possible consequences.
K
|
|
|
DavidM
United Kingdom
458 Posts |
Posted - 06 Jun 2011 : 16:49:01
|
I guess there is more to this problem than meets the eye, I've tried it but I don't get the same fault.
- New schematic with R1-3, translate to corresponding PCB.
- Add new R4 to schematic.
- In PCB, rename R1 to R4.
- Back Annotate.
This changes R1 in the Schematic to R4, first renaming the existing R4 out of the way as R5.
David
|
 |
|
|
KevL
United Kingdom
78 Posts |
Posted - 06 Jun 2011 : 17:04:26
|
Strange but in my example
In PCB I actually did
R3->R4
R2->R3
R1->R2
I.e. multiple renames.
Now back-annotate
(may be this is different from your example where perhaps only 1 item is marked for renumbering during back annotation)
In my case the R4->R5 did not happen and so I had 2 x R4
Other possibility is that I actually did about 30 renames in 1 pass (rather than the 3 in the example I gave - which was to illustrate the observed problem). Could you have a renumber buffer length type issue????
K
|
Edited by - KevL on 06 Jun 2011 17:08:08 |
|
|
|
CAEIntegration
USA
1 Posts |
Posted - 08 Jul 2023 : 16:12:21
|
Actually back annotation is severely limited. I'm making an adapter board for a tester where the pinout is completely arbitrary, so I adjusted connections to make the routing easier. Back Annotate does not understand this at all and returns "The PCB Design has no renames to back annotate." Instead I need to throw out my schematic and use the "Reverse Engineer" function.
Christopher L. Plumlee |
|
|
|
edrees
United Kingdom
768 Posts |
Posted - 08 Jul 2023 : 17:03:19
|
@CAEIntegration
Net changes in the pcb will not be back-annotated to the schematic.
The design process is generally from schematic to pcb, but if you then wish to rename the component Designators in the routed pcb in positional order for example, then the renamed Designators will transfer back to the schematic. Clue is in the words "Rename" and "Back-Annotate"!
Maybe you were expecting something different, (like "Reverse Engineer"?).
In your example, its usually easier to update the schematic manually as you change the nets (one by one) in the pcb editor being careful that you do not accidentally merge different nets together.
|
|
|
|
Peter Johnson
United Kingdom
493 Posts |
Posted - 10 Jul 2023 : 11:39:28
|
edrees is quite correct apart from one specific case. That is [Edit], [Swap Connections]. In this case (only!) back annotation WILL remember and and apply the changes to the schematic.
This function was specifically included to allow the layout to be tidied up when tracks crossed unnecessarily, as can often happen with memory routing or when multiple input gates are involved.
There are no checks on the connections being swapped so it's very much a case of checking carefully to make sure you're swapping the correct pair and not corrupting the circuit operation by accident! |
|
|
|
Peter Johnson
United Kingdom
493 Posts |
Posted - 10 Jul 2023 : 11:52:43
|
Just noticed this.
If one adds a new part in a schematic e.g. R3 and then opens up a PCB which has not yet being forward annotated (so has no R3) and one then chooses to rename on the PCB so that R2->R3, R1->R2 and then back annotates then the process will be successful.
But now there are R3 (2off) on the schematic. This is unlikely to end well.
Of course I'm only renaming stuff in the PCB and back annotating because forward annotating rips up the PCB on renames - never the less there is clearly a problem here and care might be needed that the fix does not create new problems. E.g. Cant back annotate or back annotate also renames unintended parts are obvious possible consequences.
That's an unusual and very interesting scenario which I'll log as a bug.
It's true that forwarding changes when there are a lot can result in tracks being ripped up. you can be forewarned of this by using Integrity Check first so you can see this in the report. There are two strategies now possible. The tedious one is to make the changes manually but there's a more subtle way of minimising the damage. Under [Settings], [Preferences] on the 'PCB Interaction' tab there's a 'Delete' area. Set the option for 'Delete Track Does Unroute' if it's not already set. you can then delete one segment of any affected tracks which returns that segment to a connection. now forwarding changes won't rip up the remaining track. It will simply reconnect the connections, which usually results in significantly less disruption to the tracking.
The strategy for forward planning to avoid this scenario is to avoid mixing renames and connection changes in the same operation. If you have pending track or connection changes, forward these before atempting any schematic renames. That way the topology of the pcb matches that of the schematic and the function is significantly more likey to recognise simple component renumbering as that rather than misinterpreting it as tracking changes. |
|
|
|
Peter Johnson
United Kingdom
493 Posts |
Posted - 26 Jul 2023 : 10:54:21
|
The team have attempted to reproduce this problem, but without success. For this to be investigated further, an example of the problem is needed.
If possible, please send this to <support@numberone.com> quoting DMS 54120. |
|
|
| |
Topic |
|
Bug in Back-annotation