I have managed to save a frame with a development disclaimer in Annotation for our company needs. However, I need to do that same thing in 3D viewport. Is there a way to have a disclaimer shown as default in a 3D viewport and also be able to print any designs with the disclaimer printed on it as well? Any help anyone can provde for this newby would be great.
Go to the Annotation tab.
Click the annotation plane FLAT TO SCREEN
Create the note and place it on the screen.
This will remain on the screen at all times as long as the graphics toolbar has "show annotation displayed.
If you have view states, make sure it is always displayed for each saved view.
Why cant you attach a note with a leader when using "Flat to Screen" annotative plane? This was available before Creo. Am I missing something?
Thanks for the quick response. We may be using a different releases of Creo 2, I say this because my annotation dialog box is named "Annotation Plane Manager" and your is "Annotation Plane" and the look is a little different. In any case, when I change the settings per your video it allows me to place the note on an object, but there is still no choice for a leader. Is there a parameter I need to turn on? Or any other reasons I don't get the "Note Types" menu to assign with leader. I do get the "Notes Types" menu when using any other annotation planes other than Flat to Screen.
I might have had to sneak up on it. It is not in the plane manager. This is the "Current Orientation" dialog found when you right click on the annotation. It is quite convoluted.
From what I can tell, you 1st make the annotation attached using any 3D annotation plane (not flat to screen).
You then right click on the annotation and select "Current Orientation" which will open the dialog in the video.
This pops the annotation to the origin of the part without a leader.
Then you have to re-attach the annotation and move it.
Problem is, the annotation is difficult to select (try the annotation tree) and very difficult to place.
I am on Creo 2.0 M040.
These steps helped amazingly and are exactly what I have been looking for this past week. I have been trying to create 3D notes for a while now i managed to get them placed correctly with leaders but not oriented to stay parallel to the screen or viewer so not to end upside down or backwards and always remain readable. And when i did manage to get the notes parallel to the screen or 'flat to screen' it would loose the leader. The leader is important in what i am doing. In my job I am required to update our prts library with many things including '3D flat to screen annotations'. Following your exact steps i did the following to complete the notes.
Creating a new Note
Annotate > Annotations > Notes
Name the note accordingly and place somewhere visible attached to a entity
in the model, at this point its not important where its placed beacause it will
be moved and attached at a later step.
Make sure to select from the new menu manager that appears
'with leader' and 'standard normal or tangent leader' click done and place.
Next step is to select the note just created
(L-click to select note R-click for menu options and select > Current Orientation)
You will be prompted with the 'ANNOTATIONS PLANES' menu window make sure to select everything
as shown below. This step will send or move the note to the origin of the model,
Next step is to select the note just created ones again
(L-click to select note R-click for menu options and select > Properties)
This will prompt the 'Notes' menu manager shown below.
Select Mod Attach... > On Entity and select a entity in
the model where you which the note to be place with a leader.
Select Done to complete the step
Then select Move and move accordingly. I recomend to have the model
in standard orientation before moving the note to avoid loosing it in space.
Go to View tab > and in Orientation > select Standard Orientation.
Hope this helped out.
Gabriel Ortiz Hydraforce Inc
Great work around. Thanks for the step by step. I still wonder why PTC is removing functonality and making it harder for us to do our jobs. This was a simple procedure before Creo. Why would you complicate things?
Side note: I've been using Pro-e for 15 years and they have always seemed out of touch with the little guy. Thats why Solidworks has kicked there #%&@ (with an inferior product) and made it harder for Pro-e users like us to find jobs. Look at the help wanted adds, it's very evident Solidworks users have an atvantage of Pro-e users.
I'm done venting now.
Yes, really nice!
But when I check it in to Windchill, the note does not pop up. I will contact PTC on this one or can I find the answer here?
Thanks in advance.