Inventor General Discussion

Reply
Valued Contributor
mattsons
Posts: 50
Registered: ‎03-30-2011
Message 1 of 3 (465 Views)

Smooth lofts from inside a part

465 Views, 2 Replies
04-18-2011 01:06 PM

In this dolphin i am working, i want the fin to flow smoothly into the body, the fillet doesn't look right. I have created the base of the fin inside of the body and suppressed it, then lofted them through points and a 3d spline. I get errors though, "can not create" and such, so i found that i have to extrude the inner surface to the outside of the body for it to work, but then it doesn't flow smoothly into the body. Does anyone have a suggestion on how to adjust this, how to merge the fin smoothly into the body? Thanks

*Expert Elite*
JDMather
Posts: 26,830
Registered: ‎04-20-2006
Message 2 of 3 (457 Views)

Re: Smooth lofts from inside a part

04-18-2011 01:48 PM in reply to: mattsons

I see two problems.
The first is that the profile is not smooth - tangent continuous.
The second is that the path does not end at a point in the 2D sketch (create a construction line a sketchpoint to terminate).

Please mark this response as "Accept as Solution" if it answers your question.
-----------------------------------------------------------------------------------------
Autodesk Inventor 2014 Certified Professional
Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional
Inventor Professional 2015 64-bit
http://www.autodesk.com/edcommunity
http://home.pct.edu/~jmather/content/DSG322/inventor_surface_tutorials.htm
Employee
johnsonshiue
Posts: 2,149
Registered: ‎04-30-2008
Message 3 of 3 (447 Views)

Re: Smooth lofts from inside a part

04-18-2011 02:50 PM in reply to: mattsons

Hi! Great model I must say. If I were you, I would not make the fin a solid feature. I would create a loft surface and then extend it to the main body. Lastly use Sculpt feature to create the solid fin.

On the current model, you can do the following to avoid some rework.

 

1. Thicken/Offset -> pick the Loft2 face -> set output to Surface -> distance = 0. Basically copy the face associatively.

2. Make the surface invisible.

3. Delete Face -> pick the Loft2 face and the Extrusion7 faces. You will get a solid with a hole. Actually, you will have two surface bodies now.

4. Make the offset surface visible.

5. Extend the surface toward the main body.

6. Sculpt -> pick the extended surface and the main body.

 

This is just a proof of concept. I would rework it by creating loft surface and sculpting the surfaces instead.

Thanks!

 

 



Johnson Shiue (johnson.shiue@autodesk.com)
Principal SQA Engineer, Inventor
Mechanical Design
Autodesk, Inc.

Announcements
Are you familiar with the Autodesk Expert Elites? The Expert Elite program is made up of customers that help other customers by sharing knowledge and exemplifying an engaging style of collaboration. To learn more, please visit our Expert Elite website.
Need installation help?

Start with some of our most frequented solutions or visit the Installation and Licensing Forum to get help installing your software.