How To Dimension An Ellipse In An Inventor .IDW

[sdreed52]

Our company, which sells office furniture, wants to offer an elliptical shape table. My project is to model and draw the table top. The modeling part is easy. I  just used the elliptical tool to create the sketch then extruded it to create the 3D shape.

Next I started a new drawing, placed a top view and began to annotate it and there is my problem. The general dimension tool will not select anything other than the outside shape. I need at a minimum the radius of the major & minor axis. See screenshot below.

Another post suggested use Retrieve sketch dimension, however in my Inventor (2021) I can't seem to find that option. For example, in the Edit View, under Display Options, there is no such command. Under the Recovery Options tab, there is an All Model Dimensions command that is grayed out.

So, I am at a loss as how to dimension a simple thing as an ellipse. I've spent quite some time searching this forum but haven't found anything to help so my last resort is to post here. Surely someone has needed to make a drawing of some ellipse shaped object and run into the same issue.

Thanks for your help,

Steve

[sdreed52]

Yes, you are correct, iLogic is not required to recreate the model in the drawing view. However, this is not just one table top of one size. It is several different sizes with and without power module cutouts in varying locations. The possible combinations are huge. Therefore, the engineer decided to use iLogic to model it. It works great for other shapes, just not the ellipse shape. I have no idea why; I'm just the lowly cad guy trying to make drawings. 

Thanks,

Steve

[Frederick_Law]

Yes, something wrong with your iLogic "ellipse".

Attach the file so we can check.

[Frederick_Law]

You problem is not IV cannot dimension ellipse.

The problem is how the "ellipse" is modeled.  Probably.

Unless, your drawing view is off.  Not looking directly at the surface.

Can't do anything until we see some files.

[sdreed52]

If you look at the feature tree, it appears to be a regular ellipse sketch created with the ellipse tool then extruded. I am baffled why it doesn't work. I can recreate it without using iLogic and then the dimensions works as many have indicated.

I'll look at posting the model and drawing if I am allowed, got to check that first.

Thanks,

Steve

[sdreed52]

Here are the files. I have stripped out some proprietary information. I'm sure the iLogic tables won't work but it generated the geometry in the attached part file.

Thanks,

Steve

[sdreed52]

I have attached them in another reply from LT.Rusty. Look at that one.

Thanks,

Steve

[sdreed52]

I attached the file in a reply to LT.Rusty. Take a look at that post.

Thanks,

Steve

[LT.Rusty · Accepted solution]

That's an interesting one. I understand why the dimension fails, and I can replicate the failure in a new-created part, but I'm not sure how to make it work correctly. 

Fortunately, there's a workaround.

First- the failure is because you're no longer dimensioning an ellipse. The actual sketched ellipse was used as part of a cutting operation, and the tangent points where the ellipse meets the box are where your problem comes in. I get why the part is modeled that way--you're following your manufacturing steps in the process of making the model--but it's not really the "right" way to do it purely from a modeling perspective: it leaves dirty edges, as you've discovered.

The workaround is pretty simple, though. 

You can just put a sketch on top of the view with your not-quite-ellipse in it, then use project geometry to get the "ellipse" into the sketch, then use the sketch tools to draw another--actual--ellipse over top of it. Dimension the sketch geometry, then go back into the sketch and change it to "sketch only," so that it's not visible.

It's annoying, but so long as you need to model your parts based on the manufacturing process, that's basically what you'll have to do.

[sdreed52]

I am glad you were able to figure out the "why" of the problem. I am not sure it has to be modeled that way; I'm guessing he just thought that would work and didn't realize it would "break" the drawing view.

Thanks Much,

Steve

[Frederick_Law]

No problem dimensioning the ellipse.  Even got the one with fillet.

On you drawing:

[Frederick_Law]

Your Snap Setting?

[sdreed52]

Interesting.  But, mine just doesn't work.

Thanks,

Steve

[sdreed52]

My snap settings are exactly same as yours.

Thanks,

Steve

[Frederick_Law]

The R3 fillet prevent IV from recognizing the ellipse.

I can't dimension a rotated ellipse with fillet.

Easy without the fillet.

So, use ModelState to remove fillet in drawing.

[damian.lewczyk]

Please vote for this idea:
https://forums.autodesk.com/t5/inventor-ideas/full-dimension-of-elipse/idi-p/13404028