Struggle with annotating angle dimension in drawing

[Anonymous]

Hi

I am struggling with annotating angle dimensions in drawing view using Autodesk Inventor Professional 2017.

The part in my drawing is a circular disk with 16 holes close to the edge, 20 degrees apart. When I am trying to annotate the angle, using dimension,from hole to hole, nothing is happening. I have also tried to create a sketch with the part projected, with lines illustrating the angle without any luck.

The only way I can accomplish angle annotation is to create a non-projected sketch, where I draw the angle lines on free-hand, which is quite bothersome.

There has to be a lack of functionality I am missing here, have anyone experienced the same?

Thanks

[TheCADWhisperer]

Attach your files here.

I will wager that the solution is easy.

I certainly wouldn't do a "freehand" sketch.

[SBix26]

Sounds as if you just need to use the Centerline tool to make a "bolt circle" through those holes.  This will provide properly oriented center marks at each hole that you can use for angle dimensioning.

Sam B

Inventor Professional 2017 R3
Vault Basic 2017.0.1
Windows 7 Enterprise 64-bit, SP1
Inventor Certified Professional

[Anonymous]

Still struggling.

Here's a when I try getting the dimension. It just turns blue and does nothing.

I have attached the files.

[Mark.Lancaster]

@Anonymous

As @SBix26 pointed out you need to use the center pattern annotation centerline.  No need to create a sketch..

However there's something wrong with your drawing view because even when I did the proper annotation it still didn't work.  So I recreated your base view in your drawing  and its now work.

Also just wondering why your view orientations (related to the view cube) are kind of messed up.  Meaning your base view in the drawing is based on a bottom  view.  In my opinion its not really modeled correctly.

[Anonymous]

Hi, thanks for your answer.

I have realized that this problem is present in some drawings. Do you have any idea what causes this?

And you have right, when I try to create a new drawing it works perfectly to assign angle dimension.

Is this a bug or is it a setting for avoiding this?

About the "bottom-top" comment, does this matter when the bottom is identical with the top?

[Mark.Lancaster]

@Anonymous

I guess looking at home position of the view cube, too me Its just an odd orientation.  I come from board drafting days and my base or primary view would never be based on a bottom view of a part or assembly.  Same with CAD, my primary view would most likely be based on a front view.   Anyhow my 2 cents..

[blandb]

Don't forget you can right click on the view, and select "Automated Centerlines". This works for normal views and will place the circular pattern for you. It also works for side view to place in the center line.

But if you ever change your pattern, your drawing will break. Please see link below:

https://forums.autodesk.com/t5/inventor-ideas/automated-centerlines/idi-p/5247915

It has been accepted, was hoping to see it in an update..maybe next release.

Hope this helps!

[Anonymous]

I had same problem when dimension angle for ladder with cage.  One of my college finally solved this problem by changing " general dimension type" to " projected" instead of " true".

right click mouse and choose " general dimension type".

[Anonymous]

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@Mark.Lancaster wrote:

However there's something wrong with your drawing view because even when I did the proper annotation it still didn't work.  So I recreated your base view in your drawing  and its now work.

I'm unable to download the part and drawing but I'm just wondering if his view is ever so slightly skewed and thus causing the issue? Just a thought.

But yes, draw the centerlines in as shown and then just dimension centerline to centerline.

[Anonymous]

Right click on model ---> General Dimension Type ---> Click on Projected