Unable to create Arcs or circular dimentions

[davemorl]

Hi,

I have an issue when creating a 2d drawing from my components, once i start adding dimensions to the drawing linear and base dimensions work fine. As soon as i try and dimension the holes they aren't recognized?

Is this a bug or have I personally done something wrong here?

Here is my file and screen cast demonstrating the problem

Dave

[paul.clauss]

Hi @davemorl

Thanks for posting! I think you have stumbled upon a bug with the ISO standard drawings - when I tested your file with an ASME standard drawing, I found that the dimensions were created with no errors. I've brought this up with our drawings development team for further investigation and we appreciate you bringing this to our attention.

In the meantime, please use an ASME standard drawing to work around this problem behavior. You could also use the Leader tool to manually apply the arc dimensions in your existing drawing. Please feel free to reach out with any questions.

[Anonymous]

@davemorl

Hi Dave,

did you create the drawing with view front?

If so, Fusion works as one can expect. There is an angle of 0,1° between the guide face and the XY-plane of the origin. In this case the projected geometry results in ellipses, not arc/circles. Radius/diameter dimension needs arcs/circles.

With the correct view orientation, you can use radius/diameter dimension (ISO).

You can verify it yourself:

1) do a "look at" on the face of the guide

2) create a named view

3) use this named view for drawing view

4) create radius/diameter dimensions

Manfred

angle between face and XY-origin (=TOP FRONT view)

 

named view with normal/perpendicular view on face

use named view to create drawing view and create diameter and radius dimension

[Anonymous]

@paul.clauss

Interesting observation. The (Fusion 360) ASME and ISO algorithms obviously have different tolerance values for "interpreting" ellipses as arcs/circles.

I tested it with a box/hole component created with an angular construction plane. Dimensions created at 0°, then I changed the angle of the construction plane.

Results for 0.1°

-> ASME: no warning, you also can create new diam/radial dimensions

-> ISO: warning, new diam/radial dimensions don´t accept geometry

Results for 0.5°

-> ASME and ISO: warning, new diam/radial dimensions don´t accept geometry

[paul.clauss]

Hi @Anonymous

Thanks for posting! The ASME and ISO templates do use a different tolerance, which I believe is the cause of this problem for the OP as well. We appreciate your input - I will pass your post along to the development team for further investigation.