error in Ultiboard 11 forward annotate

[rschoele]

I'm using Multisim/Ultiboard 11.  I get this error consistently in version 11.   I change or add components to my schematic and use the rename/renumber component tool.  I already started a PCB layout so I will then Forward annotate to Ultiboard 11.  In ultiboard 11 I get a list of design errors stating pins are missing from component shapes connected to a specified net.  i.e. 

Ultiboard  -  Thursday, February 04, 2010, 10:36:29 AM

Forward annotation [PLSM3750]  - Thursday, February 04, 2010, 10:36:46 AM
Forward annotation completed;  0 error(s), 0 warning(s);  Time: 0:00.19

DRC and Netlist Check [PLSM3750]  - Thursday, February 04, 2010, 10:36:53 AM
    Design Rule Error: Net 2 connected to Net LTSRC
    Pin "+" from part "C6"(2.2µF) in net "555RC" is missing from shape "32mmPolyFilm"
    Pin "-" from part "C6"(2.2µF) in net "0" is missing from shape "32mmPolyFilm"
    Pin "1" from part "C6"(2.2µF) in net "0" is missing from shape "32mmPolyFilm"
    Pin "1" from part "J2"(180Pin) in net "0" is missing from shape "180PIN"
    Pin "1" from part "R4"(4.12kΩ) in net "555VCC" is missing from shape "RESC1608X63N"
    Pin "2" from part "C6"(2.2µF) in net "LTVT" is missing from shape "32mmPolyFilm"
    Pin "2" from part "R4"(4.12kΩ) in net "555DIS" is missing from shape "RESC1608X63N"
DRC and Netlist Check completed;  8 error(s), 0 warning(s), 0 filtered error(s);  Time: 0:00.01

The problem is for example that the part 32mmPolyFilm is not, nor ever was connected to net 555RC and the same goes for all the other flagged errors.

Is this a SW bug right now or did something change in how your supposed to forward a new net list?

thanks

Ryan

[Tien_P]

Hi Ryan,

Please have a look at the attached file for reasons why you are get these errors, if this information does not help, go to ni.com/ask and create a service request, send us your Multisim, Ultiboard and your user database, we can investigate this problem for you.  If you don't know where you User database is locate, in Multisim or Ultiboard, select Options>>Global Preferences>>paths

[Beacon_Matt]

Hi all,

I have the exact same problem too.

I've tried deleting the affected parts, forward annotating, thus removing them from Ultiboard, and then putting everythign back again, yet the problem still exists.

I've run through your checklist, Tien, and I can't find any mismatched pin names.

Do you have any more suggestions?

[Tien_P]

Hi Matt

Without looking at you file it's hard to figure out why you are getting the error, if you can go to www.ni.com\ask and create a SR, send us the file and we can look at it.  You can also attach your schematic and Ultiboard file on this forum but to keep your design confidential, delete all company information, all the parts on the design but leave the problem component and maybe a few surrounding components, do the same with the Ultiboard file.

[dbur]

I have had this exact problem with almost all design since updating to ver 11.  It's quite irritating.  I have to insert all the 'missing' components, make a manual list of the nets on all their pins, then go to the netlist editor and delete them one by one.

This always happens as I work on a design and renumber component refdes in MS then forward annotate.

This has to be a bug and should be a high priority to get fixed.

David B

[Tien_P]

Hi David,

Try this in Ultiboard, select Tools>>Netlist Editor>>Pins tab, press the "Delete" button and then select all nets from the "select the net to delete" dialog" and remove them.  In Multisim, with the schematic updated, forward annotate to the Ultiboard design.  This should update the Ultiboard netlist.  This is a known issue.

[dbur]

OK, I'll try and remember that next time.  Sounds much easier than hunting down each offending net and pin.

David B

[JasonPinkham]

I completely agree Dave, this same issue cost me over a weeks worth of work.  This issue didn't show itself until I was half way through a 400 pin BGA and noticed a short between to two pins that was never supposed to be there.  After fixing the BUG, all the pins are shifted to new positions and its back to square 1.  I have never had anything close to this happen with ANY other schematic/layout package.  I can't imagine what NI is thinking here but it does seem to add up with some of the weird comments the sales person sporadically mentioned about not accepting returns on software...only accepting upgrades.

[zaba]

I have been having this frustrating problem since the upgrade. I have since rolled back to version 10. This, along with the other bugs in Ultiboard, makes Ultiboard 11 virtually unusable. Requiring every user to go through this rigmarole every time there is a change in a schematic would seem to warrant a speedy fix from NI.

[dbur]

If your problem is the same as mine on this particular issue there is a very simple work around.

Open the netlist editor in UB.

Click on delete net.

Select all nets.  (select the first, scroll down, shift-select the last)

Delete.

click OK

Now re-import the netlist and all is good.

I normally only have this issue sometimes when I've renamed a components in MS.  I'm not sure exactly what scenario of renaming causes it.  Some do, some don't.