Modelling aircraft nose, help!

Hey guys,

firstly just like to say that it looks like you've got a great and helpful community, just what I was looking for with regards to CATIA! Ok, so I'm trying to design the nose section of a commercial aircraft eg. 737 / A320 size. I've generated the sketch profile which the nose is based on. (Don't worry about the pointy end / general design of it. I'm just trying to get it to work before I start worrying about little things!) The middle line is located at 2/3 of the diameter of fuselage measured from the top.




Now when I tried to surface this I ran into trouble. My first thought was to do it in two sections, the top and bottom halves. I was going to use sweep, with two guide curves. The profile would have been the fuselage arc, one guide curve in the horizontal plane and another in the vertical. Catia refused to compute the anchor points automatically and i couldn't choose the right ones to make it work!

After this i decided to try split the nose into quarters, instead of halves. I first tried to fill the quarter. Although the fill worked, the surface was "sucked in" or depressed in the center which wasn't what i wanted.

I ended up trying the sweep with two guide curves again. This time it worked! I used the same guide curves and the profile curve was only the quarter section of the fuselage arc.



Now there's a couple of things not perfect with this solution. Firstly, you can see that it's not ideal as each quarter section bulges out and then comes in where it meets the other sections. The result, not a smooth surface between the joins of each surface. The other thing was I had heaps of trouble giving the surfaces thickness. The two top quarters I used the pad function and that worked. For the two bottom surfaces I couldn't select a direction for the pad without encountering an error.

"The profile is locally paralell to the extrusion direction. The extrusion cannot be defined at that place. Chose a profile and a direction that are not parallel."

I sort of understand what this error means. But the wierd thing was that for the two top quarters, I chose the same direction for the pad and it worked. After this I tried to use thick surface instead, and got the following error.

"Current offset value leads to a local degeneration on a surface: body cannot be built"

So that's where I'm at. If anybody could offer some advice on this that would be great. Perhaps there is a better way from the start to go about it.

Thanks!

Maybe try multisection surface with relimitation setting unchecked?
I think you'd have to add at least one more section.
You need some geometry for continuity toward the nose I think.

Catia doesn't like "sharp pointed" surfaces

Thanks for the advice.

I'll try with multisection surfaces without the relimitation setting unchecked (what does that setting do?). I always find with more complicated multi section surfaces I can't get CATIA to do it the right way, like it just tries to create a surface which turns in on itself. I've tried messing around with the direction of the arrows on each curve to some positive result. But it's mostly trial and error. Any other tips on using multi section surface? EDIT: So yeah just tried it again following your advice. Can't get it to work Always leads to a cusp! I'm thinking now just having a series of circles offset from each other and scaling down towards a point. And then multi surface them all together.

Relimitation unchecked allows the MSS to go beyond the selected sections, basically using the last section to sweep along the guide curves.  Since your guides flow beyond the section, and you can't have a section at the end point, I thought that would be a good option to try.

As far as how to use MSS, check through the help doc.

Quick advice: coupling = ratio, arrows same direction, make closing points intersections between one of the guides and the two sections

good luck!

here's another approach to your surface modeling of the nose cone:

1. since the nosecone is symmetrical, start with the curves on the port side


2. extrude the top and bottom curves in the Y direction to control tangency in next step


3. create the Multi-Section surface, based on the bottom, middle and top curves. Add tangency at the bottom and top.  Use the bulkhead circle has a guide curve. 


4. Mirror the surface and Join the two halves together.

Wow thanks Jack for your time and effort you put into the detailed step by step process. I will try your method and let you know how I go!

Thanks again.

I revolved a parabola to get the nose cone, and then did as Jack said.  It worked a champ!  The tangency for the symmetry operation was killing me previously.  Thanks!

Ok so I managed to make the surface with MSS and mirror it. BUT! Now I can't thick surface or pad it. I can only ever do one half, then CATIA spits the dummy when trying to do the same to the other Even if you use pad successfully on one half, and try mirror the pad itself CATIA just shoots out an error!

I got an error message about the pointed surface causing problems when I tried the ThickSurface. Did you get a similar error? (I'm not sure what you're doing with a Pad)

As JMCMILLANNA said earlier: Catia doesn't like "sharp pointed" surfaces

I added a Plane behind the nose point, and Spit the Joined surface with the plane. Then I was able use ThickSurface.

I'm not an airplane designer, but isn't there a spherical surface at the nose? It probably would be better to start with a sphere (or half sphere), and use it's edge as a second guide curve, with tangency, when making the Multi-Section surface.

Posted By aubzaubz on 26 May 2010 11:16 AM
Ok so I managed to make the surface with MSS and mirror it. BUT! Now I can't thick surface or pad it. I can only ever do one half, then CATIA spits the dummy when trying to do the same to the other Even if you use pad successfully on one half, and try mirror the pad itself CATIA just shoots out an error!

I had a chance to work with this after my earlier post.  I was able to convert the pointed surface into a solid by using CloseSurface.  But I was unable to Shell it to get the wall thickness.

So, another method to solve this (and I'm sure there are lots of things you could do)...

Add a Plane behind the nose point, and use the Plane to Split the CloseSurface solid. Then add a Fillet to roundoff the front of the nosecone. Now use Shell to remove the back face and define the wall thickness.

I figured out a pretty good way to do it. I used MSS. Just two circles, one circle for the larger rear end of nose and a second very very small circle at the front of the nose. Then I used four guide curves to taper the larger circle to the small circle. I made the front circle so small so that it effectively tapers down to a point. Had no trouble thick surfacing this time!