Drawing symbols disappear, why?

Question

Hi all, this is a strange one....I have a Creo 2 drawing. I can place custom symbols as free entities without problem, I can also use the "on entity" placement and this is also fine providing I select some edge geometry to place it to.However!.... if I choose to use an "on entity" placement and select the leader line of a dimension, the symbol will disappear after a few minutes. I can use the find tool to relocate it, but it's not visible or printable on my drawing.This fault occurs regardless of which symbol I choose (I have tried a few), and as a test I have created a brand new drawing, using the same model, and successfully placed a custom symbol on a dimension leader line. There must be something up with the original drawing???Any ideas?This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

mender · Accepted Answer

Another thing to check, in your old drawing, update to versioned fixes by the detail setup command update_drawing. The reason for this is that a fix that affects symbol visibility would require versioning to avoid changing the appearance of an existing released drawing on retrieval.

Workflow:

File > Prepare > Drawing Properties > Detail Options > "update_drawing" for the 'option name', and "all" for the value.

then add this symbol, and see if it now stays. If it does, then all is good, unless some other fix corrected by the update changes your drawing's appearance in a way you don't like. If that is the case, you can file an SPR to have us hunt down which specific versioned fix is the one that addressed this issue, and you can update to only that one.

BenLoosli · Answer

Check your layers.I have a drawing program in our template drawings that puts symbols on the drawing depending on drawing classification. After modifying the program, some drawing sizes put additional symbols on a hidden layer that is not active. We can locate them and then cut and paste them back to a visible layer. Never have figured out how to prevent it or to make a certain layer the 'active' layer when the drawing program exits.

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