Datum Feature Symbol

[a_valle1]

Hi, 

I am having this weird issue where a random datum feature has appeared on every single sheet I have on a drawing I am working on. This feature shows up on even sheets that have no drawing model associated with it. Has this ever happened to anyone else and does anyone know how I can get rid of this? I literally can't even click on it and it comes up on each sheet in the exact same place. Any info would be appreciated. 

[KenFarley]

The only thing I can think of is that your drawing format has been mucked about with and this symbol added to it. That would explain the "not being able to select it" aspect of your problem. You could try to add a new sheet to your drawing and see if the symbol appears again, maybe even try a sheet with no format.

[manjunathrv]

Try to add this detail option to the drawing and update the sheets

[BB_9593767]

I tried this out - did not appear to change anything.  Datum Feature Symbol still appears on all sheets after changing this detail option on the drawing and updating all sheets.

[KenFarley]

Again this sounds like something has been added to your drawing format. For example, we have a note about drawings being interpreted per ASME Y14.5. It looks like a simple note on the drawing, but cannot be selected or changed, because it was defined in the drawing format.

A way to check this theory is:

(1) Create a new sheet.

(2) Right mouse button and select "Setup" from the menu.

(3) Change the format listed to one of the blank ones, which have names like "A Size", "A1 Size", etc.

If I'm right, the troubling symbol should no longer be visible.

To fix the problem, if I'm right about the cause, you'll need to find and fix the format file being used for your drawings, then replace the format on each sheet with the fixed one. Unless someone knows an easier way to do so.

[TomU]

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@KenFarley wrote:

...you'll need to find and fix the format file being used for your drawings, then replace the format on each sheet with the fixed one.

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Replacing the format won't be necessary as long as the symbol is not contained in a table.  Tables are copied from the format to the drawing.  Everything else is sort of visible through the drawing and any changes to the format will be instantly visible anywhere that format is used. 

[sacquarone · Accepted solution]

Hello @a_valle1 

Most of the time, this kind of issue occurs:

• Already in 3D (in the Drawing Model), when a Set Datum (created in pre-Creo 4 versions) was converted in a Datum Feature Symbol in Creo Parametric 4.0 and later
• When this was done while using >Annotate >Annotations >Legacy Datum Annotations Conversion (but left with incorrect or incomplete information in this conversion process of the legacy Set Datum item)

How to proceed when issue occurs?

• In some situations, setting update_drawing all + >Review >Update all Sheets in Creo 4.0 M130+, 6.0.5.0+, 7.0.1.0+ and 8.0.0.0+ helps
• When abobe approach is useless:
  • R&D needs to access impacated data to provide a fix at data level (and for this, a new case needs to be reported to PTC Technical Support)
  • One workaround - effective most of the time, but again not awlays - consists in approaching this as follows:
    1. Create a New Drawing
    2. Ensure drawing_units in the 2D DTL of the new drawing is aligned with what was defined in imapcted drawing
    3. Use the functionality >Layout >Import Drawing/Data, and select the legacy drawing in session
       • Above process will import in the new drwaing everything which was existing in legacy one, BUT WITHOUT (in theory) the corrupted DFS items appearing in multiple seehts, and unselectable (and therefore undeletable)

Hope this helps as next step.

Regards,

Serge

[BB_9593767]

The update_drawing all method didn't work for me, but the last workaround you mentioned did!  Thanks for your help!