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How to Sweep this

How to Sweep this

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 !

Sweep_Base Lines.PNG

Sweep_Base Lines_Side View.PNG

Even if I create the section just after the selection of the normal trajectory.

Creo don't want to make the intention modeling.

Sweep_Trajectories.PNG Sweep_Trajectories + Sections_Preview Model.PNG


and it reworks the section has you can see ! 


Does anyone think HE CAN manage to make this modeling ? ?




Re: How to Sweep this

In the context of the construction geometry you have shared I would suggest using a variable section sweep. Using the trajectories shown in your picture. If you constrain the sketch  to the trajectories to maintain your design intent it should work.


There are other methods that could create this but without the context of design intent you may not get the most relevant suggestions.

Re: How to Sweep this

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.

Creo is an endless adventure: Always more to learn.

Re: How to Sweep this

You're trying to control it with too many trajectories.  This would probably be best done with a boundary blend with just the circular edge of the tube and the elliptical curve, with a curvature continuous (if possible, if not use tangent) condition used on the "tube" end, and a normal condition used on the curve end.  It appears that you care more about the cross-section at both ends, and not so much about what goes on in the middle as long as the surface is smooth, and the above method would give you exactly that.  Also, you can adjust the parameters for the curvature and normal conditions by varying the value or enabling the drag handles.

Re: How to Sweep this

Thanks for giving your comments, tbraxtonkdirthFrankSSchiavone


So find here what I have at the beginning !

Sweep_Base Lines_Originals-1.PNGSweep_Base Lines_Originals-TopView.PNG

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.

Swept Blend.PNG


@ 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.

Boundary Blend_EllipseToCircle_2.PNG

Boundary Blend_EllipseToCircle_1.PNG

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.

Re: How to Sweep this

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.


VSS setup1.jpg

Re: How to Sweep this

Here you have the original and it comes from CREO 2.0

Re: How to Sweep this

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.


ISDX Curves.jpgISDX Surf.jpg


solid model.jpg


Re: How to Sweep this

Hi tbbraxton,


Yes ! it seems what I am triying to reach, but with too many curves it doesn't solidfy,

And here there is not ISDX avalaible !


I will try again with Boundary Blend.


The other problem with VSS is that the plane where the section start is not decided by the user .... !!! but calculated by CREO and depending on the trajectories curves !!


Can you explain more ... what let you say that the VSS is not the best choice.


Thanks !

Re: How to Sweep this

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.



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