3D Annotation in Creo Parametric 2.0?

[ebeattie]

I have been trying to use the 3D annotation in Creo parametric 2.0 and it seems that it does not work.

I right click on the icon in the ribbon and select "Set". When I click on the icon to reorient to the set plane, it goes to the Top view and stays there.

No matter how many different annotation planes I set, it does not reset the annotation plane to that plane. It is stuck on the same plane.

The interface looks like it would be very easy and intuitive. but no.

Has anyone been using 3D annotation with any success?   How?

Is there any tutorial videos available?

My company would like to start doing MBD but it does not look like the 3D Annotation is working yet. Help?

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.

[Mahesh_Sharma]

Earl,

Is this an issue with one part or with all of the files?

For a quick test:

1. Select Front from annotation planes > Active Annotation plane and check for reorientation.

[ebeattie]

I think I have a handle on it. It seems that there has to be a combination state for each plane or something. I will work on it for a couple more days and see if it makes sense.

Thank you.

[sschilling]

Earl,

We are trying to do the same and increase our use of the Annotations.  One button in the Annotate tab is Update.  Try using it as a save what I have button.  See if that helps.

Scott

[ebeattie]

Thanks Scott,

I will.

[Hongjie]

Hi Earl,

one more.

'+' in bottom line of graphics window can be used to add view, (for example you can add section veiew, detail view and so on).

After adjusting the model in graphic window, you can use Annotate>Combination States >Update to save current model oritation (position).

Annotate>Annotation Planes only set plate to put your annotation (dimenstion, geometric tolerance and so on), NOT for turn (re orientation model in graphic windows). By click Annotation Planes >Active Annotation Plane can directly turn model to annotation plate setted by you.

Croe prefer you to add 3D annotation from Annotate>Annotation Features in stead of Annotate>Annotations. Of course you can use Annotate>Manage Annotations>Show Annotations to directly show some dimension before using Annotation Featrures to create them.

Our company still use 2D annotation now, they said 3D will be in future. Now I create some 3D annotation which can quickly shown in 2D detail drawing, 3D annotation is mroe convenience then 2D.

It looks 3D annotation is litter unsteadiness, some time Creo 2.0 will jump out during 3D annotation operation.

PCT has very basicly 3D annotaion online training coursePrecision LMS : Login ( not free)

I think with Creo help at Creo Parametric>Fundamentals>Annotation features, you can reach PTC on line basic training curese level. Even reading the hlep is boring things.

Best regards,

[cc-2]

Hi Earl

Since WF4 3D annotations work pretty well.  Since 2007 I have switched my users from 2D to work with 3D annotations for components and assemblies.

WF3 was OK for components but not for assemblies. Also the interest for me was to ability to view 3D models and have all the information about it (from parameters and also dimensions, tolerances,, surface finish etc...) in Creo and ProductView/Creo View.

At first glance it may appears thigns do not work. For instance, when you open in Creo View a 3D drawing, you have all the dimensions from all the components all displayed together. you can imagine that you can t read a thing. We developed methodology and created layers

eg.  ANNO_PRT for the annotation for components,  ANNO_ASM for the annotation related to assembly.

In Creo View you can then very easily switch on and off the annotation you want to display.

When you select ANNO_PRT only the annotation created in the prt files will be shown. Of course when you have several components it may still look messy too but you then isolate the component of interest.

We were able to take design decision without 2D drawings.  Of course it takes some get to use at the beginning as you need to rotate the model to see some of the dimensions, here again with standard procedure it is easy to do. Our main plane was Front, so users have to put as much as possible on the Front plane. If not possible it was Right.  Right view has a short cut in CreoView so you press it and the model reorient and you see the dimensions as per a 2D drawings.

There are situation where you can't avoid the "mirror" effect so you just press the touch to show the model the other view.

It is a very powerful tool. When you search for a product, you find the wtpart/model first. so if you have a 3D drawings, you do not need then to open the drawing.

Also when investigating an assembly you often need to go to to componet level. With 3D drawings, you stay within the same window of Creo View without the need to open 2D drawings, after 2D drawings. In 3D drawings, you just isolate the components.

Also we have used 3D drawings to generate 2D drawings automatically.  Unfortunately, sometimes we had unexepected behaviour,  2D annotations got positionned differently than 3D annotations.

All  in all. 3D drawings are very powerful and hope to convert the engineers in my new company.

I do not know the capability in Creo 3 but hope it can only be better