3D Annotations VS 3D Annotation Features

[gfraulini]

Hi all,

you can create a 3D annotation as a text with leader or a gtol, and this kind of thing is visualized at the top of the model tree.

Next, you can create a 3D annotation feature, in which you can create a set of all the annotation (gtol, finish surface symbol...)

What is the logic that guides you to prefer one way instead the other one?

What is the advantage in using the first method or the second one?

PS: I use WF5.

Thanks.

Regards

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[TomD.inPDX]

This is a very interesting question and find it hard to believe we've had no responses during the day.

I am not fond of the model annotation, but I too would like a good overview of the annotation feature's purpose.

[James62]

To me it seems like the annotation feature (2nd method) has to follow parent-child relationships, while the 1st method doesn't have to.

[gfraulini]

I'm not an old user, I work with proE only by 3 years and now I would start to explore this kind of approach to design where you put directly on 3D view the information that, normally, you put on the 2D views.

I think this gives you more awareness of what you're doing because you put all the manufacturing notes during the design, when the mind is more concentrated on the part.

I'd like the opinions of older users and also how you use it (3D notes are a bit hostile in the use...)

[James62]

I guess Brian Martin could tell us more. If he's still around.

[BrianMartin]

I'm still around...

Speaking specifically of the way this tool works in Creo 2.0 and 3.0, the primary benefit is that the annotation feature can hold several different annotations (as you pointed out). The first method is what I'd regard as the "older way" to use 3D annotations. The second method is the "newer way". Even as late as Creo 2.0, annotation features can be finicky. Some work well (GTOLS) and others do not (weld symbols).

This problem is compounded by the fact that there are several different ways to create certain annotation types. For example, I can think of 3 ways to set a datum plane (for GTOL purposes). What's worse - sometimes one method works while the others do not! This makes the entire affair challenging and, at times, very frustrating. Creo Parametric 3.0 has improved the consistency a little - but there are still multiple ways to create these 3D annotation features. There are also several functionality gaps still being addressed.

In general, Model-Based Engineering (MBE) or Model-Based Design (MBD) is the latest trend. Larger companies are investigating or pursuing this approach in an effort to reduce design cycle times, simplify product definition, and move away from paper-based documentation. The results are mixed so far - but PTC has invested quite a bit of effort into developing these tools and making them work within sister products like Creo View.

To address Giulio specifically, the way these annotations were created in Wildfire 5.0 is maddening. I wouldn't recommend attempting to use 3D annotations at WF5 unless you have a strong tolerance for frustration. Creo 2.0 is much better - but still not perfect. I'd stick with the Annotation Feature before using those pre-defined individual annotation picks. Moving forward, using the "catch-all" Annotation Feature is the way to go - so getting used to that workflow now will only help you as you move to newer releases of the software.

As to why you'd use one way over the other - at Wildfire 5.0 you'd just try all ways until you found one that worked consistently. The tool was very inconsistent and really did require numerous attempts before you'd get a satisfactory 3D annotation. It seemed to me that the least effective annotations were created using option #1 therefore I stayed away from them.

I hope that helps steer you in the right direction!

Thanks,

-Brian

[gfraulini · Accepted solution]

Thanks Brian to be intervened.

So between the "old" method (placing the symbols using the simple annotations) or the "newer" one (using the annotation feature) the only difference is that the newer unifies the simbols within the feature in the model tree instead of placing them at the top of the tree.

In addition, it is normal to have some problem in the positioning of this annotation becouse the tool starts to be efficiently since the creo 2.

Thanks

[jgeling]

Hello,

What about the possiblilty to replace reference?

In a annotation feature it is possible to replace a reference of an individual annotation. I couldn't find this possibility in the 'old' annotation.

Johnny

[Hongjie]

New one will create feature bottom of tree which is more easily to create dimension in detail drawing (2D) with already has annotation in 3D.

Old one need to choice right annotation in mass dimension.

so if you need both 3D and 2D annotation, you need at first create in 3D by New one (annotation feature) then in 2D (detail drawing) you can quickly create annotaiton by choice tree bottom's annotation feature.

Best regards, Hongjie