Academic Company Events NI Developer Zone Support Solutions Products & Services Contact NI MyNI
This Document is not yet Rated  Rate this Document

Parts Become Unplaced After I Forward Annotate

Primary Software: Electronics Workbench>>Multisim
Primary Software Version: 10.0
Primary Software Fixed Version: N/A
Secondary Software: Electronics Workbench>>Ultiboard

Problem:

I have Multisim designs that were created with version 9 or earlier. I was able to edit my design in Multisim and then use Transfer » Forward Annotate to Ultiboard to update my Ultiboard netlist with the changes.

Now I am using Multisim and Ultiboard version 10 and having problems with this. All of my old files open fine in the new versions, but when I forward annotate changes to Ultiboard I see that many parts -that had nothing to do with the changes- get unplaced from the board outline.

Why is this happening and how can I fix this?



Solution:

First, lets remember that whenever a user makes any change to the schematic file in Multisim, and these changes are then forward annotated to the layout, Ultiboard first checks any difference between the present netlist and the newly forwarded netlist, it will then unplace any part that was affected by a change. This unplacement happens for a security reason and to make sure that the user will correctly place the part after the change.

Now, on this particular problem, the root of the problem is that in earlier versions of Multisim and Ultiboard we used common footprint names. In version 10 we have now adopted IPC standard footprint names.

Here are some examples:

Common Name

IPC Name

SO-8

SOIC127P600X175-8N

SO-16

SOIC127P600X175-16N

PDIP-8

DIP8300

11-15A2

DIP12300

In version 10, the common name is still used but behind the scenes there is a mapping table that maps the common name to the IPC name.  The reason why the common name is still there is because if we used the IPC name, many users would not be able to find footprints in Multisim. 

The problem is when you open a design created in Multisim 9 or earlier. The common name is updated and now maps to an IPC name; when you forward annotate the design, Ultiboard compares the present netlist with the forwarded netlist and it sees that a new footprint name is used, therefore it unplaces the part. Even when the part is not related to any change made by the user.

To solve this issue you have two choices:

  1. Replace the old footprint name with the IPC footprint in the original Ultiboard design file to match Multisim's mapping.
    • In Multisim, look in the Components tab in the Spreadsheet View, locate the RefDes of the components that became unplaced.
    • Locate the Footprint column and for each RefDes double-click the Footprint cell to open the Edit Footprint dialog.
    • Click Select From Database to open the Select a Footprint dialog.
    • Multisim will show you the exact location of the current footprint, the Footprint column shows the common name.
    • Scroll right and find the Ultiboard Footprint column, this column shows the IPC standard name.
    • Write down this Ultiboard Footprint name.
    • You can now exit all dialogs, and repeat for every component that gets unplaced.
    • After you have all the correct names, you can now switch to Ultiboard.
    • Locate and select any of the affected parts and then select Tools » Change Shape.
    • In the dialog, make sure that you select Ultiboard Master under the Database field, also, place a checkmark to Show subtree contents. Now, place the cursor in the text field under Available Parts and start typing the IPC name you wrote previously from the Multisim footprint dialog.
    • Once you start typing it will filter all the footprints and you will finally find the correct footprint. Select it and click OK.
    • If multiple parts share the same footprint a pop-up message will ask you if you want to replace them all, you can click Yes.
    • Repeat for all components that need to have their footprints changed. Make sure that you confirm that each new footprint is correctly connected, has the right location and the right rotation.
    • You should now be able to forward annotate correctly.

  2. Each component that is using the new footprint name, can also be saved to the User Database and use the old name. 
    • In Multisim, select any of the components that are having trouble.
    • Double-click the component and go to the Value tab of the Properties dialog.
    • Click Save Component to DB. Find a proper Family and Group for the component and save it.
    • Replace the component in the schematic with the new component, right-click the part and select Replace Components..., choose the new component saved from the User Database.
    • Double-click the newly replaced part. Now click Edit Component in DB.
    • Select the Footprint tab, click Add from Database.
    • Make sure that the currently used footprint is selected and click Copy To, select the User Database and click OK.
    • Now, you are still in the Select a Footprint dialog, switch now to the User Database and locate the newly copied footprint.
    • Scroll right until you see the Ultiboard Footprint column, and with the mouse cursor and the <Delete> key delete the cell contents.
    • Click Select to map to the new footprint.
    • Acknowledge any warning message and if in the footprint preview window you see instead of the footprint a message saying Footprint not found in the Ultiboard Database, then look at the Note at the end of this document.
    • Back in the Component Properties dialog, you can confirm pin mapping and click OK to exit.
    • Save the component back in the same place, make sure that Replace Component in Circuit is checked. Click OK to exit and acknowledge you will overwrite the component, click Yes.
    • Repeat for every component showing the same problem, once you have finished you should be able to forward annotate correctly.

We recommend Option 1 since you are not modifying any of the databases, however if the IPC standard footprint size is not the one that your design requires, then try to use Option 2.

NOTE: If the footprint was not found, that means that even on the previous version where your original design was made it was mapping to another footprint. What you can do here is a very simple task:

    • In Ultiboard with your original design open, select Tools » Database » Database Manager...
    • Select the User Database and click the Add parts to the select item in the tree icon (  ) in the Database toolbar section.
    • In the Add new parts to the database dialog, select the Target Database to be the User, and check any footprint that you are missing in Multisim, click OK to exit.
    • You can now click Close and go back to Multisim, you should now see the preview of the footprints.


Related Links:

Developer Zone Tutorial: How to Forward Annotate from NI Multisim to NI Ultiboard
Developer Zone Tutorial: How to Back Annotate from NI Ultiboard to NI Multisim
Developer Zone Tutorial: Creating a Custom Component in NI Ultiboard



Attachments:
AddIcon.JPG

Report Date: 04/15/2008
Last Updated: 04/16/2008
Document ID: 4KEA33VG

Your Feedback! poor Poor  |  Excellent excellent   Yes No
 Document Quality? 
 Answered Your Question? 
  1 2 3 4 5
Please Contact NI for all product and support inquiries.submit