MERGING/COMBINING BODIES

[Anonymous]

Hi

I am struggeling to make a part consisting of four reflectors that merge into a top plate. I have drawn a profile of what is to be a led reflecor and revolved it. I need 4x of these, so I used a rectangular pattern.

Problem 1: I have spaced the reflectors such that the inner surfaces are +-0.2mm apart. The outer surfaces protrude into one another. How can these protrusions be removed (see four reflector.png).

Problem 2: What I need to do is draw a rectangular sheet 1mm thick and merge it with the the 4x reflectors. The top of the sheet being flush with the top of the reflectors and the bottom of the sheet meging into the curvature of each reflector. In other words the plane in "four reflector plane.png" needs to extrude downwards following the curvature of the 4 reflectors

Is there a way to do this?

Thanks.

[JDMather]

What version of Inventor?

Attach your *.ipt here.

I would Revolve only the outer face of the reflector and then Shell.

Several ways to do the planar feature, I might give it a try if I knew what version of Inventor.

http://home.pct.edu/~jmather/content/DSG322/Inventor%20Tutorials/Inventor%2011%20Tutorial%205.pdf

[Anonymous]

Thanks for the reply. I'm using Inventor Proffesional 2011. I have attached the part of which I have done a rectangular pattern of 17.1mm spacing

[JDMather · Accepted solution]

I told you incorrectly - using the Ice Cube Tray Tutorial from above -

Revolve Cut only the internal volume from block and then shell.

I noticed that your Sketch1 is not fully constrained - which is poor modeling practice.

http://home.pct.edu/~jmather/SkillsUSA%20University.pdf

[Curtis_Waguespack · Accepted solution]

Hi hendrix777,

You can use a bit of trick to help with your model as well.

• Here I've created one Revolved feature.
• Tthen I shelled it.
• Then I created a pattern using the Pattern A Solid option.
• Then I created the top "plate" feature with an extrusion.
• Then I added fillets to the corners

And then the trick:

• So at this point I dragged the Shell feature down below the fillet feature, in order to have all of the "holes" created.

Attached is an example model created in Inventor 2010 (I don't have Inventor 2011 any longer.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[Anonymous]

Thanks guys. Helped a lot