Error when trying to put angle on a section view

[WillL84]

I'm trying to put an angular dimension on a section view of a part. I had no issues doing this on this exact same part in Inventor 2015. I can add an angular dimension to the non-sectioned view (see red circle) but when I try to do the same dimension on the sectioned view I get a leader that shoots 28937538 miles off the top of the page (red arrow). Any ideas?

[CCarreiras]

All the files are yet migrated to the newest version?

Sometimes, when some files are migrated and others have not yet, can arise some odd behaviors.

Also, make sure you have all the updates installed for the version you are using.

[WillL84]

The files are latest, all updates are in. I actually took the old file and saved it with a new part number (making slight changes) then made the changes and now I'm doing a brand new drawing for it.

[CCarreiras]

I did a quick test... is working:

Could you share the files to test?

[WillL84]

Unfortunately I cannot share the files. I did whip up a test part like yours and it worked fine for me there so maybe it's still got something linked to the 2015 file version.

[CCarreiras]

try to do a dummy file and check if the problem persists.

[johnsonshiue]

Hi! This may have something to do with default dimension type. Go to Tools -> App Options -> Drawing -> Dimension Type Preferences -> click on the Radius button on the right -> click on Angular dimension.

Many thanks!

[WillL84]

@johnsonshiue thanks for the suggestion but that didn't work. I think it's got something to do with the file originally being created in Inventor 2015 and now it's been modified in Inventor 2023.

[mikegreslick6607]

What are the chances that the section line / section line sketch isn't snapped precisely to the center of the part? I can definitely replicate your behavior with a section line that is offset just a tad.  In the below, Section A-A is snapped to the exact center of the part and provides proper behavior, while Section B-B is offset just a few thousandths of an inch (actual dimension is irrelevant here) and yields the behavior that you're seeing.

[WillL84]

I thought you were onto something so I deleted the section view and added a center point to the main view so I'd have the exact vertical points to redo the section view but it's still doing the same thing. I'm going to try redrawing the part from scratch in 2023 and see if that fixes it.

Edit: doing a revolve then extrude didn't work as the revolve gives a perfect point and this model can't go that way lol.

I did notice that if I click on the angled line as the start I also get a gigantic radius like you show in the rightmost image. 6,762.033 inches to be exact lol. Now I made this part using a loft command. The right end is round and the left is a rectangle. I used loft to connect the two surfaces with the "free" condition for both edges. Maybe it's got something to do with the loft and the section view? I'll try redoing it as a revolve then just extrude the rectangle into it and see if that fixes it.

[johnsonshiue]

Hi! On a cone, the cut edges are linear only when the section plane passing the center axis. Any slight deviation will lead to a parabolic shape.

If possible, please share the files in zip here or send it to me directly johnson.shiue@autodesk.com. I would like to understand why the angular dimension does not work properly.

Many thanks!

[WillL84]

I just shot an email over, thanks. I did check multiple times to make sure that the section cut was dead center and it is. I even used the center point mark on the body to be 100% sure.

[WillL84 · Accepted solution]

So for anyone with this issue in the future - in an email exchange with @johnsonshiue he suggested to create a sketch on the drawing, project the line and then draw a line. Then you can reference that sketch in your dimensions. I wasn't even aware you could sketch on a drawing!

[johnsonshiue]

Hi Folks,

Without disclosing the specifics of Will's model, here is what I found. The model edge of interest here is spline. It is not linear. As a result, the linear dimension does not apply here. In order to dimension the edge, adding the sketch line to the drawing view can help.

Many thanks!