Wrong values for radius dimensioning

[jonas.andersson3538Q]

Hi,

I have a problem with radius dimensioning of a spherical surface done with lofting. 

When I are in the General Dimension command it shows one value, R393,3. After locking the dimension position it changes to R290,2. If I make a Three Point Arc as a sketch connected to the geometry the dimension will be R393,7. This also the correct value that it should be according to the calculation we use for the lofting parameters.
(also shown in attached picture).

Any ideas why this is happening?

It is very worrying if we cant trust the general dimension values.

We are running Inventor 2019.5.1
I have tested in Inventor 2023.1.1 and the behavior was the same.

BR

Jonas

[kacper.suchomski]

Hi

The geometry created with the Loft method is a spline, not an arc.
You can overwrite the dimension value in the drawing if you need to.

If you want to create an arc there, change the modeling method.
Create a sketch with an arc and Revolve to create a solid.

[johnsonshiue]

Hi! Kacper is right. The loft edges are spline edges. In theory, the spline's radius can vary. Inventor approximates it as an arc within certain tolerance.

Many thanks!

[JDMather]

@jonas.andersson3538Q 

I am surprised that nobody has mentioned to Retrieve Model (sketch) dimensions in the drawing.

[SBix26]

I'm not an expert on geometry, but I can't see how the surface of that lofted solid could possibly be spherical.  It's very nearly cylindrical on one side (below left), and something more approximating a sphere on the opposite side (below right). As others have pointed out, it's not precise analytic geometry, but rather a spline face. 

I think your only recourse is to fake it in the way that @JDMather recommends (dimension an arc in a sketch in the part and retrieve that dimension in the drawing).  Or, if it is supposed to actually be a spherical surface, model it so that it truly is spherical.

---

Sam B

Inventor Pro 2023.2.1 | Windows 10 Home 21H2

[jonas.andersson3538Q]

Hi all,

Thanks for the replies.

I realize now that I was a bit unclear in which view the image with dimensions was from.

Regarding the geometry, in one of the axis the contour lines are part of a circle. i  I made a section in the attached picture and got one more value for this radius...

@kacper.suchomski  
Maybe this is a spline but in the actual view, and section, this would be parts of a circle.  I cant create it as a revolved arc as I need to change the diameters for the lofting circles and where the centerpoint for those are placed. We have  made a program for calculation of the values to use.

@johnsonshiue  
In one exact plane/section going through the center it is a fixed radius.
I tested this in an other CAD software and it handled it correct. Maybe they have a better algoritm for approximation  of the spline? The third radius value in the section make me even more worried.
Can this approximation also have effects on a step file?

@JDMather  
Retrive dimensions from the ipt do not work in this case as this dimensions are not included in the lofting feature