SolidWorks & wings

[Anna Wood]

Chuck,

Did you get the model I sent you? I will have time to post on some other techniques on my blog over the weekend.

Cheers,

Anna

[zx32tt]

I got the model you sent. Thanks for your efforts. I'll check out your blog.
Chuck

[Spooky]

Hi, new guy here.
I thought I'd throw these pics out there to give you an example of lofting in SolidWorks... I like to sketch the outline of the wing and use that as a guide curve(s) to connect the airfoil sketch's, that way you get the wing shape you want and not some funky, twisted mess. One tip when lofting with guide curves is make sure your airfoil sketchs intersect with the guide curve(s); use the pierce mate where the airfoil and guide curve meet, makes life much easier.
First pic is just the sketch's...Second is after lofted, and third is how it looks in place.

[Mithrandir]

canopies are always fun... how would you do a 3 bounday surface in SW?

[Spooky]

	Quote: Originally Posted by Mithrandir
	canopies are always fun... how would you do a 3 bounday surface in SW?

For the canopy, I usually make a solid body close to the shape I want, then trim/fillet the shape to my liking and shell it out to whatever thickness.
As far as a 3 boundary surface, you can extrude it, or use separate sketch's and loft it, then use the thicken feature to get your desired thickness .

Yeah, I haven't made the canopy on the above model yet, it still needs finishing, but that one is pretty easy to make, unlike a Bearcat canopy with that funky bubble shape... that one needed a little more thought.

Hope that helps.

[Mithrandir]

	Quote: Originally Posted by Spooky
	For the canopy, I usually make a solid body close to the shape I want, then trim/fillet the shape to my liking and shell it out to whatever thickness. As far as a 3 boundary surface, you can extrude it, or use separate sketch's and loft it, then use the thicken feature to get your desired thickness . Yeah, I haven't made the canopy on the above model yet, it still needs finishing, but that one is pretty easy to make, unlike a Bearcat canopy with that funky bubble shape... that one needed a little more thought. Hope that helps.

I have done it several times in Pro/E... I was just curious what capabilitie SW had???
There is a trick in Pro/E to do it.... basically two nested 4 boundary surfaces with tangency.

[Spooky]

Never used Pro-E myself, but I learned CAD with Unigraphics, then went on to SolidWorks... There's probably a lot of similar features between the two, just named, or used a little differently. That's the way it was between UG and SolidWorks, although UG has more options on the way things were done, especially in SolidWorks early days.

Here's a pic of my Bearcat made in SolidWorks... Still more detailing to do on it.... I tend to have more than one project going on at a time .

[zx32tt]

I've gotten the wing lofted, and a couple of spars in place. I have reference planes at the places where I'd like to have ribs. How do I create a sketch of the rib on a sketch plane using the existing surfaces ? If I view a cross section at the ref. plane, I can not convert entities. I could do a cut-extrude thru at each rib station, to create the needed edges, but that seem like a lot of added effort. Suggestions please

[Spooky]

Hey zx32tt,
Looks good... make a sketch on each Rib plane you have and try using an Intersect curve on the sketch for each section, where the sketch plane and wing surface meet.

Let me know how it works out.

[zx32tt]

It worked! But, I still need to get better at this. I would like to create the sketch on the new ref plane for each new rib. Can I just click on the ref plane and insert new part, the create the sketch using intersect curve?

[Spooky]

Yes, you can.... and that way each rib is it's own Part file and keeps relations to the wing too, and if you change the wing later on, the ribs will change with it.

Good luck and keep me posted.

[zx32tt]

the way I'm having to do it is create a sketch on the ref. plane, by using the intersect curve, clean it up, and do a copy-paste into the new part. I haven't been able to create a new part sketch without going thru all these steps