Section line = Radial line + curve

[FilipeMais]

Dear all,

I need to draw a section view of a circular part with many holes on it.

The holes as the configuration that you can see in the pictures bellow (They are the same part).

In Inventor 2022 I just can use the Section line B-B (bellow left) but I would like to use the Section line that I sketched (bellow right).

When I select the sketch with the desired section line

(radial line + curve) appears the error message bellow.

Can anyone help?

The projection I want should just consider the green lines

[CCarreiras]

Hi!

It's possible to do it in Inventor 24, but be aware that it will sum all the branches in the final section view:

[NigelHay]

Wouldn't you get the same section result if your arc was a horizontal line? (assuming that part of the flange is solid). You might have to draw the angled part of the section line in approximately the right place then edit the section line sketch afterwards.

[Rory_M]

Probably not the answer you were hoping for but I think 2022 was limited to straight lines.

2024 will do it, and allows arcs in the section line.

If you compare the arc (B-B) versus straight (C-C) in the image below, you'll see that using straight lines only distorts the view so you can no longer trust the dimensions.

Using 2024 and a section line with an arc gives you the result you need.

Section views

[mluterman · Accepted solution]

After years of having this "issue", I finally came to this conclusion (and it definitely works the exact way you want it):

Rules for getting a revolved section view without issue:

1. To start with, you can’t have any other dependent views on that sheet (face view only). Otherwise, any changes to the “section cutter line” may result in a truncated section (incomplete cut and section line).
2. See screenshot below:
3. a) All line segments must point to the center of the part (see green dashed lines).
4. b) All arc centers must lie on the center point of the part (not shown).
5. c) The very last line segment near the “D” and OD of the part must exist and pass through that “quadrant” (actually the midpoint of the jaw segment as shown). If you simply let it trail off the part (marked in red), you will get the wrong dimension in your section view since the dimension at that location is not the part’s true radius (actually, radial distance in my case). >>> THIS STEP MAY NOT APPLY FOR A FULL/COMPLETELY CIRCULAR PART; I HAD 3 INDIVIDUAL PIE SEGMENTS THAT MOVED TOWARD CENTER IN THAT FACE VIEW <<<
6. d) All line segments must “sweep back” to that last line segment once you finish the sketch (like looking down at the top of a door hinge as you close the door).

[SBix26 · Accepted solution]

It works in 2022 also.  Here is my demonstration attempt.  I think the key is what @mluterman wrote, that the lines must be carefully constrained to be coincident with the center of the arc.

---

Sam B

Inventor Pro 2024.1.1 | Windows 10 Home 22H2

[FilipeMais · Accepted solution]

Dear Inventor Users, Mluterman, SBix26, Nigel_hayphotek_co_uk,  Roy_M & Ccarreiras,

With your help get what I wanted. Thank you.

I hope I did understand it well.

In the following lines I share how I did it:

1) I created the view in the left and I projected its to the right and in the most right I created an independent representation of the part.

1)

2) I used that independent representation in the right to create the section view. Just with straight lines

2)

3) I edited the section view line. I drew an arc using the points already defined and I defined the constrains I needed. (I had to repeat the process and at second it worked.)

3a)         

 4) Here it is!

4)

Once again,

Thank You!

Kindly,

Filipe