Hi All
I am trying to create a cowl for a model aircraft. I have created the solid based on lofting across 3 profiles. The first and last profiles are derived from a drawing and and intermediate profile is generated and used to get the solid shape to generally match with the drawing side and plan views. However when I attempt to shell it there is an error. Lofting between first and last profiles creates a solid that shells as expected.
Any suggestions?
No chance. Clean, tidy and concise? No.
Red and purple so close together means it is almost a crease in that area.
No history, so can't manipulate the mapping handles to try and fix it.
Geometry is not constrained, blue lines, and no black ones,
way way way way too many spline points.
Using so many spline points makes a smooth curve comb impossible to manipulate.
This curve may be an Arc, not checked.
However when using two point splines and adjusting the handles to suit the trace, is giving Fusion half a chance to get you there.
3 profiles in the same sketch, is not recommended.
Your cowl will work better with two profiles and Tangential Rails, as needed.
One sketch per profile., Sketches for Rails , top bottom, then left right, so 4 sketch all together. Use Project Intersect, for the 2nd pair of sketches, or the Rails not connected error will jump out and frustrate you even more.
Curvature Comb checking is available in edit sketch mode.
Curvature mapping (coloured test) is under Inspect Menu. Zebra strips, are also under that menu.
Might help.....
The problem's probably because you have no tangency constraints. Why have you got history disabled, makes it hard to edit and see how you've made the loft.
You are going about this the wrong way, you should create three planes for each section, then fully constrain all sketches. Bad tangency between segments in the profile will stop you shelling, filleting etc. As you have it now in one sketch will mean you can't use dimensions and some constraints don't work on geometry not on the XY plane of the sketch.
In the second profile you also have an overlap. How were these profiles created, they don't seem line Fusion splines.
Mark
Mark Hughes
Owner, Hughes Tooling
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Clean geometry will Shell.
The profile shapes are causing the near creasing, sorry about that, but not really a Loft error.
Your profiles / rails are curves and ellipses.
Your file edited.... will be attached on next message, cant do too much at the same time tonight....
Might help...
Thanks for the reply.
As I said above I'll start from scratch and work through the points raised. I will need to go back and learn more re tangential and constrained sketches.
@HughesTooling wrote:
In the second profile you also have an overlap. How were these profiles created, they don't seem line Fusion splines.
Mark
In answer to the specific question I found using scale function on a sketch returned a curve described with a few points rather than my multi point spline, even using scale factor of 1.00 as a direct replacement for the digitised shape. I don't actually know what the curve is but it was generated in Fusion starting with a digitised spline, I haven't imported anything.
Reworked it today. The different approach to curve generation was a pro tip for me and really sped up the digitising.
As pointed out there was a curve well represented by an arc. Tried approach of 3 profiles in loft to start, in 3 independent sketches. Lofted and shelled without a glitch. Did a couple of iterations adjusting the mid profile to get the shape to match, no errors appeared.
If I get time tomorrow I'll try approach with additional rail sketches.
