How to annotate multiple overlapping hole features?

[Anonymous]

If I have multiple overlapping hole features, how do I annotate this in the Inventor drawing editor, i.e. *.idw editor, without multiple leaders? Currently I had to annotate each hole feature individually as I do not know of another way. I cannot hide the unwanted leaders either. Here is the example below:

I am running Inventor 2014 SP2

[brendan.henderson]

Very confusing to the drawing reader.

Can you show an enarged view to add some distance between the leabers/notes? Can you create a section through the round part to separate the leaders/notes?

[Paul-Mason]

Click on the Detail button

in the Place Views Tab

That will then, after selecting the appropriate area etc, give you something like this in your drawing

The scale of the detail is independent of the drawing that the detail is based called out from so the detil view can be set to any scale you like

Or you can just increase the overall scale of your drawing, and if nessassary use a large sheet size and scale setting

[Anonymous]

Thank-you for your response. I understand how to make a detailed view. My issue is that I have multiple features of the same type. Each feature is comprised of multiple holes. I want to refer to the feature in my drawing rather than each hole/thread within the feature. If I were doing this with a hole table I have the same problem. Inventor labels the holes indvidually, There is no way for me to combine the holes descriptions to label only the feature:

[Paul-Mason]

Edited 04-02-15 @ 1`7.15 

So this is ALL one feature of the part ???

Then I personally would edit the first hole note to contain all the information in one hole note :-

The section view just I put in to show where/how I got the information.

[Anonymous]

Thanks! That is the style of annotation I wanted to achieve. I can do this, but, now the notes are just plain text and not associated with the actual 3D model as they were originally (i.e. since orignally, I used the "hole and thread" annotation tool). If I change one of the hole definitions in the 3D model (.ipt) the drawing (.idw) will not update the annotation to reflect the change. This introduces the possiblity of drawing errors in the future. I wanted to keep the associativity and still achieve this result.

This is what the manual says about this associativity:

http://knowledge.autodesk.com/support/inventor-products/learn-explore/caas/CloudHelp/cloudhelp/2014/...

• When you add hole notes to a drawing view, the diameter, depth, thread dimensions, and other data from the model are used in the note. If hole features are changed in the model, the hole notes update when the drawing is updated.

[blair]

I would do what you did in your sample but have the Dims radially spaced farther around the hole or use a Detail-View to enlarge the area in question to allow for better detail of which arrows are to which hole along with the side section view.

You are correct to avoid manual entered text as this becomes un-associative and won't update should the model change.

[Paul-Mason]

There may be a workaround to a) keep them associative and b) Laid out as in your original post

Create a new dim style with the leader line"Arrowhead" set to  none and white line then text unchanged by using the two different styles this can be done

first showing the first dim line in "Inch"

Then the other lines whit the leader set to whit, in this example "Copy of Inch"

I've attached the to files that I used hopefully the dim styles etc come with/in them (IV 2015)