Airfoil points

[knightzero3d]

I recently imported points for an airfoil into CATIA V5 via macros and now the problem i'm having is I want to make it to a solid piece but when I go to sketcher mode, I can not use the spline function since it will not let me click on the points. How can I connect the points to form a close body to form a solid part? And is there an easier way to make it into a solid part without manually connected each point with a spline line? There must be an easier way! Thanks!

 

[Albigger]

When inside the sketch, project the points into the sketch, then you will be able to pick them to use with the spline function.

Or,
Swith to GSD workbench and use the spline tool.

--Jay

 

[knightzero3d]

Thanks for the comment but when i tried what you suggested, the spline line does not stay within the points (as you can see in the picture attached). Did I do something wrong?

 

[ferdo]

Hi,

http://www.catiav5forum.de/wbb3/wbb...44&h=606f0279935af045f68d0aee0333f16d86eed01a

Regards
Fernando

 

[Azrael]

I wouldn't use the spline from a sketcher, use the GSD spline instead and if the points are on a plane use work on support and then the spline feature.

Work on support is like a sketcher on steroids, it can be applied on curved surfaces. When a support is active all wireframe functions like line, spline etc will be set on the support. So the wireframe function will be easier to apply with a dimension less.

 

[tbuelna]

knightzero3d,

Before you import the point dataset, make sure all of the points have a common Y-coord value (as shown in your sketch). Then create a plane at that Y-coord dimension in CATIA. You can then use GSD to create a 3D spline through the points that is supported on the plane.

Also make sure that the point set in your spreadsheet is listed in order along the curve, so that they will be sequentially named and ordered when they are created in CATIA. That way you can select the points easily in the tree by highlighting, instead of having to select them one-by-one on the screen.

If you wish to make a solid from this curve, it must be closed. You can still make a surface from an open curve.

Good luck.
terry

 

[jagodragon]

sorry but i disagree with them, about making the spine on a suport that is. If you just create it thru the points it wil be more stable and have greater odds of not failing on a replay or update of the part. if you are looking to have a flat profile to create an extrude fro m then you should create the spile and then project it on to a plane, then extrude. it is an extru step but well worthit if the points need to change due to new scan data or supervisor "sugestions"

 

[itsmyjob]

to jagodragon

I think you mean SPLINE not spine or spile...

If points are to be updated (because of new value) then curves will also have to be re created because:

1 it is faster to create a 'new curve' on 20+ pts than to change definition of 'old curve'
2 once 'new curve' is built just do a replace on the 'old curve'
3 all constructions (surface or solid) using 'old curve' will now be redirected to 'new curve'

Personally I would create surfaces from 4 areas of points: Leading edge, trailing edge, pressure face, suction face.
If I had the choice I would use FSS not GSD to create curves (not sketches) and surfaces.

Eric N.
indocti discant et ament meminisse periti ​