Creating Paraglider Wing, Inventor 2013

[robo_147]

Hi I would like to start off by saying I'm new to CAD modeling, I am trying to creating a paragliding wing in inventor and its being giving me a massive headache. 

I will try and draw the best picture I can with regards to my problems but, being a newbie I'm not totally sure I'm going about things in the right way.

What I have worked out so far, generating a wing profile sketch and thats about it. 

Now for my problem. I want to position the wing profile onto an elipse shape, and rotate each wing rib to a specific angle (a tangent of a point on the elipse) .

Problem 1: First of all I cant seem to find an easy way divide the elispse in a specific number of segments. I realy just want a number of points I can then snap each profile to. (I have found the retangular pattern is able to do this but its a very round about way)

1 drawing a sketch of the elipse "sketch1"

2I then sketch circle "sketch 2"

3 retangular pattern it onto the elipse. 

4 draw a copy of sketch1 ---> sketch 8

5 project geometry of my circles onto sketch 8

6 use the center points of patterned circles as my snapto points.

Problem 2:

The angle of each wing profile changes across the curve. 

For a simpler (easier to visulise example)

If you take a half circle and divide it into 4 segments, Ie you have 5 points. The first profile will be at the horizontal (as will the last). The middle profile will be virtical, and the remaining 2 will be 45degrees left and right of the center line. 

Thats easy now do that but on an eliplse or a non uniform curve and segment it x number of times.

My wing is probably going to have between 20 and 30 profiles half that if you use the mirror tool, but still. 

Thanks in advance!!

[admaiora]

It 's not the right shape to begin with a cad software.

Using surfaces can helps you, for example and/or lofting.

It depens too on the level of accurancy you want reach. Didactic? real project?  A parachute/paraglinder has measures that need to be observed.

[WHolzwarth]

Look here for a sample:

http://forums.autodesk.com/t5/Inventor-General/2015-Part-quot-Ghosting-quot-in-assembly/m-p/5143636/...

[robo_147]

I know the file I provided has very little resemblance to a real paraglider. It was more a breakdown of steps to create a wing. Like I mentioned above this may not be the right way of going about it. I will explain more of the steps in my head ie what I'm trying to get inventor to do for me. I will attack a paint file so look at that to get an idea. 

1: Sketch elipse (and or spline for more complex shapes). 

2: divide top half of curve in = segments. 

3: draw a line through each point at a tangent to the curve. 

4: draw a line starting at each point perpendicular to each line in step 3.

All the above steps are just to get the geometry for me to attach a profile shape. 

5: generate profile 

6: attack x number of profiles to the sketch generated above. 

7: [Theres no 7 in example] basically loft profiles to generate surfaces.  

Ok the reason why I am trying to do it this way. If I can get these 7 steps to work. I can basically change the curve, change the number of profiles, change the profile shapes and get an infinite number of paraglider wings, thats what CAD is all about isnt it!!!! The model is for generating a paragliding wing surfaces in 3d then unfolding them into plan for for printing and cutting nylon so i can make a miniture real paraglider of my own design.

 There are wing generating software packages online that ether can produce the shapes I want and is far too expensive for me (its aimed at professionals) . or is a kite building program that does not really offer the shapes or parts I desire.

[wimann]

So after re-reading this post more thoroughly, I realize that the stab I've taken at it might not be quite what you need. With that said, I've attached it anyway. The only thing I can't really do with it is quickly change the number of segments. You'd have to edit the sketch, delete a constraint or two, add segment(s), constrain, edit feature and so on. It could definitely be done, but the way I have it wouldn't let you do just by changing one number.

The result you desire makes me thing this ought to be done as a sheet metal part and not as the normal standard .ipt. I don't know too much about sheet metal parts but I think it could create your segments based on a user input. Maybe someone else on here might have more information to help out with that.

[Curtis_Waguespack]

Hi robo_147,

I think you'll need to do a bit of programming to get the ability to add segments quickly and easily. Here are some quick example files that have some iLogic in them to update the parameters and segment numbers. Just download the file and then save it to run the iLogic rules and update the model. It's a bit rudimentary, but should give some ideas.

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

[wimann]

Nice iLogic. I was wondering what that would look like since you have to create new line segments each time.

How would you set up your iLogic to rename each work point / work plane so that their names are always in order? In other words, so that it doesn't skip all the ones that has generated before?

Additionally, why pattern the work plane? Don't you only need the point?

I think that does it for my questions for now.

Thanks,

[Curtis_Waguespack]

Hi wimann,

You're exactly right in that the workplane isn't required in the pattern. And really the first workplane is not needed at all, as I could have just used an origin plane or the sketch endpoint to create the first workpoint. Just simple oversights on my part as I rushed through the model creation and code trying different things.

As for the workpoint names, they can be renamed as part of the iteration through the workpoint collection.

 Attached is an updated version of the model.

'look at all of the work points 
'starting with  workpoint 2
'note that the center point is workpoint 1
i = 2
For Each oWorkPoint in oWorkPoints
'Turn off workpoints
oWorkPoint.Visible = False
Try 
'create new line segments in the 3DSketch
'connecting between each workpoint
oSketchLine = oSketch.SketchLines3D.AddByTwoPoints(oWorkPoints.Item(i), oWorkPoints.Item(i+1))
'rename workpoints
oWorkPoint.Name = "WP_" & i -2
Catch
End Try
i = i+1
Next  

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