Attach text to view

[adam.gracanin]

In drawing when I create text which describes some view it is not attached to it. Text is free. Many times I move view and text stays.

It would be nice to can attach text to view like sketch.

Example: Click on view to select it and then create text. When text is created it is attached to view and when you move view text moves too with view.

Thanks

Adam

[jletcher]

This is an easy one.

 Use leader text click on edge of the part enter text, delete leader, text will always stay wiith view now...

 Hope this helps..

 Good luck..........

[jletcher]

Just a thought if you make this a symbol and put smart tags in it you would not have to fill out the information it will take it from the part.

Also with symbols if you place the symbol in the view box then move it to the location you want the symbol, it too will stay wit the view where ever you move it..

Good Luck..........

[adam.gracanin]

Thanks a lot - trick with deleting leader is perfect

I understand your second post but dont know how to achieve it - this will also be very helpful especially since I do a lot of parametric parts.

Can you explain it a little bit more?

Thanks

[Dan_Margulius]

You can do this now. 

Pick a view and it becomes green then select Sketch command from the ribbon. 

You can write whatever you need in the sketch environment and finish.

Now your text will move with the view.

Dan 

[adam.gracanin]

Thank you Dan

uh

I totally forgot that Inventor has a text option in sketch

this is time saving too

thank you 

[dan_inv09]

I had a symbol I placed once and it somehow grabbed the view - I wanted it pinned to the page border.

You'd have to export any parameters you needed - does your symbol get sick if it's looking for parameters that aren't in the part? What if you have multiple parts on the same drawing? What if you want parameters from a part in an assembly?

I seem to recall that deleting the leader didn't stick all the time, have you tried moving the view after closing and reopening the file? Also if you use properties or parameters it will forget what it was pointing to.

I once had to resort to a leader style with a white leader and no arrowhead.

There are workarounds but they could still look into making it better. (Maybe an "invisible" leader?)

[jletcher]

Dan_inv09

 When a symbol is placed in the red view box it links the symbol to the view, even if you move the symbol out of the view box. I have never had an issue with leader text not staying with view after deleting the leader.

 No my symbol will not get sick if the information is not in the part it will not show up is all.

If you have multiple parts on a sheet using symbol with leader viz off works you attach the leader to the part and it will take information from that part only.

 If you want a part parameters that are in a part in an assembly you do the same as above leader with viz off. But this does not work for sub assemblies it will only grab parts. There is an Idea out there for an option to grab sub assembly parameters..

I have used this from day one of symbols and never had issues but one. Sometimes if you change the information in the part the symbol would not up-date unless you moved the symbol but with ilogic set to update drawing on open or change I have not had this issue.

[jletcher]

Adam,

  To start if I was you look into symbols to understand them 1st.  Next to get information from part when making the symbol the one thing you have to remember is you must have a part with the information placed in a drawing. I have no idea why it is like that but it is.

  After you have the part with that information you can make a symbol.

Here are some scrren shots to help.

With the part in you can see the things you can grab.

By click the X it put the parameter in the symbol Here I grab a custom parameter LENGTH.

Next I want the part number so I change from custom to Properties-model

Below is after I saved the symbol and inserted into drawing with the part.

Hope this helps...

[adam.gracanin]

jletcher 

it helps a lot

very useful info

thanks

[Anonymous]

I've also found it easy to just change the name of the view and turn it on.

[dan_szymanski]

Multiple solutions provided by the community for this request. Thanks everyone!

[shawn.payne]

It would still be nice to be able to right click on the text and click attach. Similar to attaching a detail to the part.

[CCarreiras]

Agree.

Place that in the Idea Station!!