3D impeller 1

[tgmcg]

I'm trying to model the vanes on a 3D unshrouded centrfugal impeller.

The disk & hub is a simple revolve.

Ideally, the vanes would be a thickened lofted surface whose profiles are simple straight lines normal to a 3D spline guide curve on the revolved face of the disk. Unfortunately, SW doesn't seem to be able to do this.

I can draw the 3D spline on the face, but cannot draw simple straight lines normal to the revolved surface, even when using multiple reference planes along the curve. I cannot seem to sketch points at the intersection point between a reference plane and a line normal to it.

Any and all suggestions are welcome.

Regards,

Tom

 

[TZellers]

Are the vanes double curvature, i.e Francis-type? That gets a little tricky. If not, or in other words if they are of single curvature, it can be done. Post which type of vane and I'll explain how I've managed to work it out.

 

[mjcole]

You might try making axes normal to the surface through points on the 3d curve and sketching lines with a coincident to curve and colinear with axis constraint.
You also might try doing 3d sketches if not already doing so and try to add points in space and giving them relations to put them on the 3d curve and on a plane in space normal to the curve.

Michael

 

[TZellers]

One of the things you learn quickly with these "mid-range" MCAD programs is how poorly they handle true 3D input. The majority of it is simple thickness controls of 2D geometry.

I've tried the surface and thicken approach, which may work depending on the geometry invovled. In my case, the vane profile was extruded from a plane normal to the axis of impeller rotation and the shrouds were created via revolutions. Clean-up was required via sharing the shrouds sketches to cut-revolve.

I guess a high end program like Nx, CATIA or Pro/E with add-ons might do it.

 

[pugap]

Why don't you draw your blade profile (as if you were looking at the blade axially) in another plane or on your backplate, then do an extrude to next surface operation to the profiled surface?

 

[TZellers]

pugap:

In most vane operations, it isn't that simple. The intersection of the vane profile is different at the front shroud versus the back shroud. Therefore, the open "eye" of the impeller would normally not be present and the vane has no surface to terminate, unless of course, you close the front shroud and add a second revolve cut to open it.

In an ideal world, you could project the vane/shroud intersection onto each shroud and do a loft, controlled as necessary by guide lines.

 

[FEH22]

I'm looking for information on how to design a Francis vane impeller. It sounds like you guys might be knowledgable in this area. Can someone point me to a good reference that gives the specifics of the Francis vane geometry? A search for "Francis vane" brought up your thread. I hope you don't mind me "scavaging" off it.

 

[tgmcg]

Ideally, I'd like to be able to handle double curvature.

One approach I've tried is to construct a lofted surface between a series of radial lines, each intersecting and normal to the axis of rotation. The intersection points are spaced along the axis of rotation to suit, as are their respective angles about the axis of rotation. A revolve cut is then used to establish vane height profile w.r.t the axis of rotation. A reasonable looking impeller can be modelled in this manner.

However, while this may suffice for "marketing" purposes, it will not suffice for engineering purposes.

SolidWorks will not allow constructing lines (loft profiles) normal to a surface and intersecting a 3D curve on that surface. This would be another interesting way to go if it were possible.

 

[pmlapl]

The mid-priced modelers don't do well with complex surfaces and shapes. However, this may work for you. Using the Top and Front planes, draw the top and front views of your blade in 2d. Create an exact center line of each sketch and use them to extrude two surfaces that intersect each other. Generate a 3d curve where the two surfaces intersect and you will have the 3d centerline of the blade. Create planes normal to the 3d curve at a spacing you think best and then sketch the cross sections of the blade on the planes. Use the loft command to create the shape. Depending on the graphics engine in Solidworks you may get a relativly accurate shape. You may have to play with the number of cross sections.
Good luck.

 

[APPENG]

Another thing that you can do without having to create the surfaces and the intersecton curve is to create the sketches like he said on the front and top planes, then select INSERT/CURVE/PROJECTION then use the "Sketch onto sketch" option and it will create a 3d curve the same as you had with the intersection curve with half the steps it took to get there.



Regards,
Jon
jgbena@yahoo.com

 

[Theophilus]

And, new in 2005, is the Curvature Continuity for loft and sweep features. The surfacing capacity of SW is improving, and is much better in 2005.


Jeff Mowry

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.