adding an arrow to a flag note

[dbolden]

It has been a while since I used Creo 2.0.  What toggle do I need to turn on to enable an arrow with a flag note? 

[TomD.inPDX]

Edit attachment on the annotation, if that is what you're thinking.

A free floating annotation can have it's attachment edited.

[dbolden]

On another drawing, when I go to Symbol/Custom, placement has: free, with leader, vertex....  Not sure how I got it to include With leader.  I believe it was a toggle within Config.pro but not sure.

[mender]

Presuming this flag note is a symbol instance.  Take a look at Annotate tab, Symbol Gallery, Redefine, <the symbol>, Attributes.  If only Free is checked for Allowed Placement Types, you may wish to define left and/or right and/or radial (if it has a circle) leader.  They'll prompt you to pick a place in the symbol definition that the leader will go up to.

[TomD.inPDX]

Symbols are not simple annotations, so Matthew is right.

Symbol definitions have "allowable" leader options.

Someone could have removed the "leader" option from your custom flag note.

Could these be intended to be simple stamps on a drawing that does not allow leaders?

[dbolden]

I have the option on other drawings I have created.  I just cannot remember what I had to turn on to get it to show.  The drawing that I am revising did not previously have flag notes.

[StephenW]

There is no toggle, either the symbol was defined with the ability to add a leader or it was defined to not have a leader.

If the option for 'WITH LEADER" isn't there, you can add it like Matthew said above (sometimes not an easy task)

[mender]

Another thing you can do, if this version of the flag note doesn't have leaders defined, and some other drawing does, *and* it is important that this one match that one:  In the drawing where the symbol is defined as desired, Symbol Gallery > Write.  In the drawing where the symbol is defined in a way you don't like, if the symbol is not in use, Symbol Gallery > Delete, then bring in the right version.  If the symbol is in use, Symbol Gallery > Redefine > Browse for the file.  It should give a dialog asking if you want to update the existing symbol and instances.  If it doesn't, change the version (the # in 'note_sq.sym.#') to a larger number and try again.  (Yes, I understand that does not work as a proper indication of version of the sym def.)  This will replace the no-leader form of the sym def in your drawing with the better one from elsewhere.

[dbolden]

What you described earlier was how I had to do it on a drawing by drawing base's.  For some reason I "thought" I had to change a toggle in config.pro.  Thanks for the help.  I will try your suggestion above too.

So I can "Write" and it will make that the standard any time I bring in my custom flag note?  It is a pain to always have to redefine and select the attachment point.  Does Creo 3.0 or 4.0 fix this?  I was not involved in setting up our standards.

[mender]

I don't know based on the information provided how the drawing came to have an ... old? version of this symbol definition.  If it is just in a drawing, you can fix it in that drawing.  If it is made from a template, and the template has the old sym def, you want to fix it in the template.  You should examine your workflows + start models to see where this is coming from.

I am reasonably sure there is no bug here as such, just that someone set up a flag note that only allowed free (and maybe on-item?) placement.  That is a fine and legal way to design a symbol.

[TomD.inPDX · Accepted solution]

I'm sure it has already been said, but this is worth noting:

You can modify symbols on the fly within a drawing without affecting the master symbol.

Most likely, that is what is happening.

You have a symbol in your library, and on occasion, someone modifies it on the fly only for that drawing.

That is actually not a bad concept but if leaders are allowed, the symbol should be updated in your library.

In environments that I've worked in, the lack of leader meant that it was never suppose to have a leader.

Adding one violates some corporate control freak's vision of what a drawing should look like.

And of course, some yahoo will do it anyway...

...and you have someone like yourself asking the very question as expected

That tells you the kind of organizations I've working in, doesn't it.

[dbolden]

I will modify and save the symbol with the leader arrow as an option.  That is done through the "write" command of the Redefine?  I believe Matt covered that above.

This is off topic but why doesn't my color change on a drawing dimension when I go into the dimension display and choose the text color?  On my system the text should be yellow and it prints as black.  I have a couple dimensions that I brought in through the Show Annotations that are maroon and purple and want to print that way.  I went into each of their displays and made sure that it was yellow but they do not update.  I even tried regen.

[TomD.inPDX]

Purple means it is not properly associated.

Maroon means you just fixed a purple dimension's attachment.

Regen will fix the maroon (should) and purple needs the attachment redefined.

Driving dimensions should never go purple (model dims).

Driven dimensions will loose their attachment on geometry changes.

Pen tables can change the plot color of a feature type.

I'm sure there are others in config.pro or even the monochrome setting in the print dialog.