dimension fillet radius

[Joonoo]

I'm pretty sure this is something very simple, but I just couldn't find out how to do it. I'm adding dimensions to a drawing and for some reason when I try and dimension the radius of a fillet nothing happens. The only time it gives me a radius/diameter is when I dimension a full circle.

[Joonoo]

Here is a picture of the radius I want to dimension

[JDMather]

Attach the file here. Have you installed all Service Packs? Did you create the part in such a manner that the curves are actually splines rather than arcs?

[Anonymous]

You will most likely need a "Cross Section View to get your Radius Dimension
of the fillet.

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"Joonoo" wrote in message news:6324857@discussion.autodesk.com...
Here is a picture of the radius I want to dimension

[Joonoo]

No I have not installed all service packs. I will do that immediately. No I did not create this part/drawing. This was sent to me as a 3D model and I made it into a drawing format to put dimensions on. Will installing the two service packs fix the problem?

[zma1013]

I don't quite understand what the other guys are saying. It should be as easy as selecting Dimension, and then simply clicking on the radius that you want dimensioned. Can you post the part?

[Joonoo]

I would take a cross section and try it out but then it will have a different radius because it has a 1.5 degree draft angle.

[Joonoo]

Yes, it should be that easy but it's not working. Sorry, I don't think I can post it up for proprietary reasons.

[zma1013]

The draft angle is most likely the culprit. You see, because of that, in the view you are trying to dimension the fillet, makes it so the arc is not a circular arc.

Forgive my terminology, the best way I can explain it.

The dimension ability only works if you are looking directly into the arc, which would make it truly circular.

I have attached a picture of what I can only guess is the problem. Looking at the top, a fillet is placed on a normal corner and you can dimension it fine. However, as you can see on the bottom, the fillet has been placed on a drafted face, which in the straight on view, makes it so the curve is not truly circular. The dimension ability will not work on stuff like that as far as I know. You may just have to do it with a regular leader in fill in the value yourself. Edited by: zma1013 on Jan 26, 2010 2:23 PM

[JDMather]

> I don't think I can post it up for proprietary reasons.

Does the part pass Inventor Quality check (green checkmark in browser)?

As I suspected in my original post the geometry is probably being seen as a spline rather than an arc.

Without the file it is hard to say. You will probably need to become very familiar with the Construction Environment.

[Joonoo]

I think you're right. You and JD are telling me the same thing. I guess for now I'll just have to use a regular leader and fill it in myself. Thanks zma1013

[Joonoo]

Yes I think you are correct JDMather. For now I have used a generic arrow and filled the header in myself. Thanks for your input

[JDMather]

Can you attach the original part here - there might be a way to fix it.

Oops, just realized that you already indicated proprietary.

Try this workaround.
Click on the view to make active and hit S on the keyboard.
Project Geometry and select the "arc", right mouse button select Done.
Sketch an arc three points (beginning, end and some third point on spline, you might have to add a coincident constraint).
Exit sketch and now you have an arc to dimension to. Edited by: JDMather on Jan 27, 2010 3:00 PM

[Anonymous]

I think JD is correct that the draft angle is the problem. The resulting
geometry in the view is probably not a circular arc but is a spline. When
attempting to create the dimension, we check if the selected geometry (the
probable spline in this case) is actually circular. If it fails this
circularity check, then no dimension will be created.

I hope this helps explain the situation.
Tim
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"Joonoo" wrote in message news:6325463@discussion.autodesk.com...
Yes I think you are correct JDMather. For now I have used a generic arrow
and filled the header in myself. Thanks for your input

[thijnvanheijnsbergen]

Sorry for my bad English and the late reaction.
First you have to select the fillet with centermark then you can select the fillet with dimension and it will give you the radius dimension.