I have a rib profile sketch that I have on layer 1 and on layer 2 at 15" away I took the original sketch reduced it by 10% to get a completed wing. Now I need to get a sketch of 5 cross-sections to get my patterns made of ribs along the wing. I tried placing planes at 3" intervals to give me 6 rib patterns then did a section view. I thought since the section was taken at a plane I could sketch on that plane by projecting the lines created from the section cut but it seems I cannot do this. Is there another way to get rib patterns made without doing incredible amounts of math going from 10% reduction at 15" what is the reduction at each individual 3" mark moving along the incline?
Solved! Go to Solution.
If you open the view manager RMB on a section view name, you can create curve from x-section. You can then use that curve to create your new sketch.
If I understand correctly you have two profiles, one at "full size" and one on a parallel plane, 15 inches away and at a size of 0.90 X the first one. You're trying to define a bunch of equally spaced "in-between" sections.
A possible way to do this is:
(1) If you haven't already, create a solid feature or surface between the two sections.
(2) Pick the surfaces of the solid or quilt, then the plane of interest for a section.
(3) Once you have picked these bits of geometry, the "Intersect" item on the ribbon under the heading "Editing" will become available. Select that, and a curve will be created with a name like "Intersect 1".
(4) Do the same for each of your planes.
Hopefully the geometry created will be sufficient for your needs. It's going to generate a single curve for each section, so you might need to make intersections for each individual surface (i.e. pressure side of airfoil alone as one curve, then suction side as another). Otherwise it tries to blend the two to make a smooth curve, with weird curvature, etc.
I went to the View Manager (Creo 4.0) and it worked. I never knew you could click on the sketch name and RMB and have a menu show up with options.
Thanks for the help.
I will try your steps and see if I understand you correctly.
To you and Stephen, why when I have sketch 1 that has interior circles for cavities and then sketch 2 is identical just reduced scale of 10%, the blend feature only reads the actual outline and blends everything external? Just a curious question.
If you are using the Blend feature, it only allows one loop, so you can't have internal features.
Maybe I'm misunderstanding your question.
You understood me correctly. So if I do another blend for the internal sketched object will the blend remove that material?