Autodesk Inventor

[#1]

Hello everyone,

I am having trouble creating an extrude-cut from an offset ellipse.  It seems that when the ellipse is offset, it becomes an associative spline.  I need it to remain associative with the original ellipse. 

But, when I try to extrude a profile using the new spline, it won't recognize the edge.

I can't just create a new ellipse, as it's profile won't quite match the offset one.  I tried tracing over the ellipse with a spline, but it then requires a vast amount of dimensions to constrain it all together.

I'm trying to extrude-cut the red outlined profile (including the elliptical part of course)..

Here is the part.  I am working in Inventor 2009.

Thanks for any ideas,

Joe

[#2]

When you offset an ellipse there are two possible solutions

1. offset equal distant - not a mathematical ellipse (usually better to Shell feature rather than offset spline).

2. True ellipse offset (seldom used - depends on where you click the ellipse to offset.

The two different solutions might not be easily noticed depending on the ratio of the minor and major axis.

see http://home.pct.edu/~jmather/skillsusa%20university.pdf

[#3]

---

jstraub78 wrote:

Here is the part.  I am working in Inventor 2009.

---

oops, see Tip 34 pg 11

http://home.pct.edu/~jmather/skillsusa%20university.pdf

[#4]

After experimenting a bit with your part  - I think you might have found a bug.
To know for sure I would have to recreate from scratch in 2012 to see if it can be reproduced.

[#5]

If I offset where one of the axis is present, I think that is treated independantly from the original ellipse.

I need to maintain the same offset distance around the entire ellipse and the offset ellipse needs to react to changes made to the original ellipse.

So, I offset the other way, which I believe creates an associative spline instead of an ellipse.  I don't think it's mathematically possible for it to stay as an ellipse and maintain the same offset the entire way around.

Did you mean tip #32?  If so, I believe I want the ellipse on the left.

Hmmm...I'm not sure if it is a bug or just something I'm missing.  Is it possible to save a part created by Inventor 2012 back as a file that I could open in 2009?  Maybe I'd be ok if I had a template part that works that I could tweak/apply my dimensions to. 

I went to Penn College for CAD, but it was pre-Inventor days....('97-'99).  For what it's worth, I can still make a mean 3D Solid Model in AutoCAD...

Thanks for any ideas,

Joe

[#6 · Accepted solution]

Did 2009 have the Sculpt tool?

Not sure what you are after - but I extruded the ellipse as a surface midplane (I used 5" but distance doesn't matter as long as it goes through the part.

Shared the sketch and extruded the lines midplane by same distance.

(eariler could not trim the elllipse with the lines)

Extend Surface the two edges of the second extrude beyond the ellipse.
Sculpt - Cut the volume between the surfaces.

You might want to check out the surfacing tutorials in my signature.

[#7]

or this?

[#8]

---

jstraub78 wrote:

 ....I can still make a mean 3D Solid Model in AutoCAD...

---

What is this "AutoCAD" you speak of?
Is that what they taught in the last century?

[#9]

Wow, I'm not very versed in working with Inventor Surfaces, but your figure/explanation taught me something new today!

The first option you have listed is what I was trying to achieve. 

As for my AutoCAD comment....well, I did prefix my statement with "for what it's worth..."  I figured I'd leave that open for interpretation  

Thank you very much for the help, this was turning into a bit of a roadblock for me...

Joe