Dimensioning Angles In An .IDW

[vertical horizons]

I created a plate that has holes in it. While in an .IDW, I want to dimension the angles between the holes.

I change from the DRAWING VIEWS PANEL to the DRAWING ANNOTATION PANEL, but I can't seem to find where I would dimension an angle.

How is this done in Inventor?

Also, I would like to be able to show & dimension the diameter of the construction line circles that I used to position the individual circles. How do you show the construction line circles in an .IDW?

(This drawing will be going to a fab shop, and they will need the specs to be able to build this plate.)

[JD Mather]

You did not need to create a detail view (section line off part) to create a Projected view.

You can Retrieve Sketch(s) from ipt or

click on the viewport to highlight (red) the boundary.
Hit s on the keyboard to start a sketch within the view.
Project Geometry and select the edges you wish to use as reference.
Right Mouse Button and select Done (this is important - different than in ipt sketch environment).
Sketch in any additional reference geometry you need snapping to projected geometry (like bolt circle) or angled reference lines.
Click Finish Sketch to get out of sketch mode.
Dimension as desired.

[JD Mather]

Or better yet

select the Centered Pattern centermark tool

select the large central hole
select each smaller hole in the same circle selecting the first hole also as last in pattern. Right Mouse Button Create.

You can now dimension both angle and pattern circle.

[JD Mather]

If you are going to use shaded views see Step 110 in this document
http://home.pct.edu/~jmather/AU2006/MA13-3%20Mather.pdf

if you don't wan't them to look like they were colored in with crayons.

[JD Mather]

Better increase the precision on the dimension for the 21° angle.

Might add a note rather than dimension 17 Holes Equally Spaced on Ø7.65 (might need to increase the precision on the Ø7.65 as well)
are you sure you have them where you want them?

[JD Mather]

For the "off vertical" angles I think I would do the section with the cutting plane through center of top view and then Center line Bisector to define the center line of the angled holes. Same for large hole in center and then simply dimension the angle.

I would demonstrate on your drawing, but without the ipt I can't edit the drawing.

[vertical horizons]

Thank you for suggesting several different options to my problem.
I am sure that one of them will work.

Better increase the precision on the dimension for the 21° angle.

Might add a note rather than dimension 17 Holes Equally Spaced on Ø7.65 (might need to increase the precision on the Ø7.65 as well)
are you sure you have them where you want them?

For the time being, this is where the holes need to be. Since water is the only thing that will be passing through the plate, the minute difference in degrees will not be of any major concern.

I will let you know shortly how the dimensioning came out.

[vertical horizons]

Or better yet

select the Centered Pattern centermark tool

select the large central hole
select each smaller hole in the same circle selecting the first hole also as last in pattern. Right Mouse Button Create.

You can now dimension both angle and pattern circle.

Thanks, JD.

That's what I needed.
Works like a charm. (It's like a magic trick. Seems kinda impossible until you know how it's done.)

You did not need to create a detail view (section line off part) to create a Projected view...

I had to show the section line because the powers-that-be wanted to have it shown on the drawing. I explained that it was not necessary, but they wanted it on there anyway.