Cutting material from revolved feature

[Cblack14]

Hey guys,

I am a high school senior and am doing a thesis on airflow around a wingtip and I am testing various wing tip devices too see how they affect the flow.  I am using Autodesk CFD, and the way I am testing wings is by using a revolved domain.  I have a half egg shape, with a wing cut out of it.  The half egg is set to be air, thus the air flows around the wing.

My questions stems from reolving the domain and having it cut out the exisiting wing.  I want to be able to build my wing and tip model (which may have some complex corners and fillets) and then create a spline and use the revolve tool to create a solid half egg while removing all existing structure.  I am pretty sure I can do this with an extrude tool, but I am having trouble doing it with the revolve tool.  I am just looking for an easier way than to create the domain then cut away at it; that approach is tedious and has created some inaccurate models.

I attached two pictures for ease of understanding. You can see the revolved domain, and then a picture of the wing itself.  The wing root is adjacent to the flat side of the domain.

Thanks in advance!

Charlie

[Cblack14]

Anyone have any ideas?
When I try and revolve it a full 180, or makes a mirror image of the wing since it gets in the way of the revolve.  I also tried doing 90 degree revolves from each side which made the correct shape, but the CFD software did not like it.  I need it to be one solid peice.  Unless there is a way to join two peices to make it seem as one?  An assemble maybe?

[JDMather]

You are far more likely to get a response if you attach your *.ipt file here.

When I read this I'm not sure if your question is about Inventor or about CFD?

[Cblack14]

Thanks for the reply.  My question is about Inventor.  Specifically creating a part that will be put into CFD, but i suppose that is somewhat irrelevant.

I have had luck creating my revolved feature and then relofting all of the wing, this cutting it out of the revolved domain.  However, I fear that when I get into creating complex wingtips, this will no longer be a viable option. My question is is there a better way to do this so that the revolve can simply create a hollow area where the structure was previously.

Attached (I hope) are my wing, and a wing/domain using the reloft procedure above.

[JDMather]

It is not clear to me what you are attempting, but I suspect the solution will involve multi-body solids and maybe Combine Cut (or Intersection).

This allows you to have multiple solid bodies within one part file and Combine, Cut or Intsect the bodies.

Each solid body can be made up from as many features as needed to model the desired geometry.

Another alternative is the use of Derived Components.

Open the attached *.ipt file.

Expand the Solid Bodies (2) folder.

Right click on the Wing and turn off Visibility.

Right click on Domain and turn on Visibility.

[Cblack14]

My end goal is to have a revolved half egg shaped solid with a hollor area in the shape of the wing I want to be testing.  Preferably, I would like to be able to make the wing first then revolve around it.  However when I try this, it leaves a mirror image of the wing (I will attach an ipt of this)

I am just trying to avoid creating a revolved half egg and then cutting away from that.  Unless you think that would be an easier approach?

[Cblack14]

OK yes! The ipt you attached is pretty much exactly what i want it to look like. A solid domain and hollow area where the wing is.

Now how exactly do you do that?

[JDMather]

As you reverse-engineer what I did - I recommend you recreate from scratch as there is some "sick" (pink) geometry in your file.

I didn't take the time to fix the geometry.  And fully constrain (dimension) everything.

[Cblack14]

That was pretty helpful, thank you very much for taking the time to help me. How exactly do you tell it to combine two solids into one peice?

[JDMather]

Everything is in the browser.

I recommend you set this project aside and go through these.

http://home.pct.edu/~jmather/SkillsUSA%20University.pdf
http://inventortrenches.blogspot.com/p/inventor-tutorials.html
http://wikihelp.autodesk.com/enu?adskContextId=HELP_TUTORIALS&language=ENU&release=2014&product=Inve...

[Cblack14]

Thanks. I will take a look at those. I consider myself to be fairly adept at using Inventor. I have been using it for a few years now and I have just never run into a problem like this.

[Cblack14]

I tried recreating your model, and i ran into a problem.  I cannot get it to revolve without cutting out the area around the wing.  Not sure how to remedy this or a way around it.

[JDMather]

You have two closed profiles in Sketch4.

Inventor has automatically selected the outer closed profile - you must select the inner closed profile or it will be left as a void in your Revolve feature.

Edit the Revolve feature.

Make the Profile selection tool active and then select the inner profile to add it to the Revolve.

[Cblack14]

When I do that, Inventor merges the revolves into one single solid body.

[JDMather]

Attach your file here  - as is - with your undesired merge, so that I can see what you are doing incorrectly.

[Cblack14]

Ok! So after playing with it I finally got the results I wanted.  The only difference between mine and yours is that you have 2 solif bodies but I only have 1.  This should be alright for my purposes.  I combined the wing and domain using a cut tool.

Here is my version of your example.  It should work for my needs.  Thank you immensley for your help and time.  I really appreciate it!

[JDMather]

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Cblack14 wrote:

 The only difference between mine and yours is that you have 2 solif bodies but I only have 1. ....

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When I did mine with the Combine-Cut I selected the option to keep the Toolbody (wing) and simply turned off the wing.
My goal was to preserve both parts rather than consume the wing in the Combine feature.

[Cblack14]

Ahh gotcha.  Well thanks!
Also, as a tangent, I ran into a problem when I tried usint my version in CFD.  The peoblem is that it is a single shell.  CFD needs it to be two halves front and back.  Your version is like this, as is my attached one.  Is there a reason why sometimes it splits the shell into halves and other times it doesent.  In my attached file, I created it the same way as I did in the version two posts up I believe.

[Cblack14]

Edit: I think I figured it out. I need to make each half with an individual spline, not a single long spline.