Hello Masters Creo Modelers,
Here in CREO 2.0 M080 ...
In the many topics about Sweeping, i have never found Sweep so straight and short ! ! !
After many tries with Sweep or Sweep Blend, there's not a good surface created by these functions.
I manage to create something with Boundary Blend but it is not enough smooth as I want.
This is the base of the problem. Sweep the ellipse (5x3.5) to the face of the solid !
Even if I create the section just after the selection of the normal trajectory.
Creo don't want to make the intention modeling.
and it reworks the section has you can see !
Does anyone think HE CAN manage to make this modeling ? ?
THANKS FOR YOUR HELP ! !
Don't know exactly the output you are looking for. Following 5 curves is difficult. The result probably would not be circular in the middle.
A swept blend would give a nice result if it fits your needs. Here is an example:
I had to manually divide the end sketch to get the arcs to line up correctly and made the result tangent at one end and perpendicular at the second.
Thanks for giving your comments, tbraxton, kdirth, FrankSSchiavone
So find here what I have at the beginning !
As you can see, it is not juste a circle at the end of the solid.
And in side view (first message) the lower curve doesn't arrived normal to the plane of the ellipse.
The long curve is made of line ┴ to ellipse plane + arc tangent + arc tangent ┴ to the solid.
@ tbraxton
With Variable Section Sweep, even if i select one of the 3 planes for Direction X or check X to the second trajectories (the lower curve) on the list, or begin on the solid face :
the creation section appears like this !
It is not on the ellipse plane or on the solid face.
so it will give the same result preview as shown on the first message.
@ kdirth
With Swept Blend, the trajectories and the sections have the same number of elements (the lower curve was divided in 3), the ends still in free :
the function doesn't show a preview ... so it means it is impossible.
@ FrankSSchiavone
With Boundary Blend and simple curves like ellipse to circle and 2 ellipse as trajectories arriving normal to ellipse plane and circle plane, let me go the end of the creation and obtain the solid.
But as I said on the first message, the first boundary I make with too many section also on the middle lets make the surface ... but don't want to solidify.
I think the difficulty comes near the lower curve that doesn't arrive normal to the ellipse plane.
One colleague I have meet and many posts or tutos tell that Variable Section Sweep was the best way but here the issue seems hard to solve.
See this picture for something to try using VSS. Create a curve along the center of the section as it will be swept between the proximal and distal ends of the sweep.
I could tell you more if I had them model to look at. If you do post the model it must be in Creo4 or earlier for me to open it.
After looking at the model, VSS is not the best choice. Your existing geometry is not conducive to VSS. I have built it using Style curves and boundary blends in Creo 4. I added these curves and used them in addition to your existing geometry to build the surfaces.
I have included a neutral file that you can open in Creo 2 in case you do not have Creo 4.
These pictures show the curves and 4 sided surface built to solidify the geometry. If you do not have ISDX module you can use Creo surface to achieve the same but it will likely take more features.
The proximal and distal sections have a geometry that are not suitable to use a single variable section sweep with the geometry you have currently. You can try to subdivide into 3 VSS which might work. Break it down as I show below for the BB construction.
I was able to use 3 boundary blends to get close to what you want. If you need tangency then you will have to do some work on your curves to get it. You will also need to make sure the quilts are normal to the mirror plane to avoid a crease in the middle of the part when mirrored. This general approach is what I would use if I did not have ISDX.
Not having your actual geometry, I eyeballed it. Using both loops as-is resulted in a weird "pinched" area on the bottom inside surface, leading me to add more control to stop that. I made one B/B (boundary blend) surface from the vertical centerline plane of the part, assigned continuous conditions to the ends, and normal conditions to the Front datum, then simply mirrored and then merged it. I didn't bother making a solid.
What I did that was a little trick I learned, was that I could have used a datum curve on the Front datum and simply assigned a curvature continuous on both ends. But I don't like that because you can't specify HOW "continuous" it is. That's why, I added features 12 thru 15. This way, I can add a B/B to use as a edge and use the extruded layout surfaces to be continuous to, and use the drag handles (Constraints tab, "Display Drag Handles") to pull the shape into what I want, something you CAN'T do with a simple datum curve. I use this technique a lot when I want more control. I could have cleaned it up more in the area of the solid itself, but I think this illustrates the point.
