Hi, I'm under stress once more...
For a new project, (single layer metal core board), I would need to add zero ohm resistors to cross tracks where necessary.
So i started my layout, and where necessary, I placed 1206 and 0805 zero ohm resitors instead of tracks.
This gives some DRC errors which I ignored..
Then I tried to back annotate this to Multisim (I'm using V10.1) using the log file...
I got an error that this couldn't be done, and the log file was deleted as well?
Apparantly it is possible to delete parts in the layout, and have them deleted in the schematic (I tried that)
But I can't add a part in the layout and have it placed in the schematic?
That's only partially back annotation, isn't it?
How should I proceed?
One of my next tasks is to reverse engineer a two layer board with some 150 components, of which no data is available.
I had hoped that the back annotation would be usefull here...
Does anyone have any tips on how I should do such a job with good results?
Johan, very stressed once more
Solved! Go to Solution.
I apologise for the long message.
Unfortunately Multisim v10.1 and prior had limited back-annotation functionality. Changes in Ultiboard were recorded to the log file that you mention. During back annotation, Multisim would attempt to re-create those actions in Multisim, and finally would delete the *.log file. In 10.1 and before, we did not support the back-annotation of new parts.
In 11.0, we re-designed our annotation system to circumvent those limitations. The new process features a "diff" between the open design (schematic capture or layout) and the file being annotated. This gives you the ability to view what changes would be made, and choose to either proceed or over-ride the proposed actions.
To speak to your specific scenario, any given footprint in Ultiboard can map to 0 or more components in Multisim. When you place down a footprint in Ultiboard and back-annotate, the annotation system will either select the associated Multisim component (if the choice is unambiguous) or provide the opportunity to select a component from the Multisim database. This component will then dynamically be placed and automatically wired up in Multisim.
If the Multisim component (linked to the Ultiboard footprint that you're interested in) doesn't already exist, I would recommend creating it and linking it to the Ultiboard land-pattern first before attempting to back-annotate. This gives you the opportunity to make sure you get the component to footprint mappings right. While we do support this scenario, we generally don't recommend that people back-annotate part additions without first doing the component creation and mappings up-front.
The latest version of Circuit Design Suite includes an evaluation period. I'd suggest you give this a shot and see if it can address your scenario.
To address your next task of reverse engineering 150 components. That may be a little tricky. The auto-placement and auto-wiring that we included in Multisim was designed to accomodate incremental changes in a design. So for example, let's say you added an additional feedback resistor in layout and attached it to two ends of an opamp. During back-annotation, we look at the placement of existing components and nets and do our best to choose the "right spot" based on the net connections that need to be made. This works well for a few components. However, trying to back-annotate an entire design will likely lead to a pretty messy schematic.
The key here is to keep in mind that any given Ultiboard footprint could map to any number of Multisim components. For e.g., an 8-pin SOIC could be mapped all sorts of different kind of components in Multisim. So you'll need to do the legwork of associating Multisim components to the footprints in question up-front in order for the annotation system to know that components to add when back-annotating into Multisim.
Here are my recommendations:
1 - Upgrade to version 11
2 - Create Multisim components and verify the component-to-footprint mappings for all the footprints in your Ultiboard design
3 - Back-annotate this Ultiboard design to a blank schematic in Multisim. If the component work is setup, then the choice of Multisim components should be unambiguous for all Ultiboard footprints
4 - Forward-annotate this exact schematic to look for any discrepancies between the two designs
5 - Clean up Multisim schematic
Hope this helps.
Thanks for rthe reply and the info.
For reverse engineering, I agree that the schematic might be pretty messy after a back annotation...
The most iportant is that connections are correct...
On an electronic worksheet, moving parts is easy...
Doing it by hand would take a few itterations before the schematic looks decent...(and hopefully correct)
I will try the evaluation version of V11.0 when the project starts.
I'll also need to contact NI to have a quote for an update... (and speak to the boss 🙂
For the metal core pcb, I'll need to route it and check out what nets need to be interupted with a zero ohm resistor.
That will be the best way for now.. there will be max 5 to 7 of those resistors to be placed...
then change multisim schematic and forward annotate...
thanks for the help!