revolve a bent solid

[Manifolddesigner]

Hello,
Got a tough one. Customer makes turbines. The blades are very curvy things. He needs to rough this thing on a lathe. I've got the model, but now I need to be able to get a 2d profile of what it would look like if it was revolve around its axis. The blades are ugly curvy things and convert entities won't work.
I've tried making a plane that bisects the blade pretty close, then doing a parting line feature on it. From there I can do some lofted surfaces that use these 3d edges as guide curves and eventually get a 2d profile. And all this just gets me close, but it's not perfect.
Did I mention they *need* to hold 0.0002" tolerances?

Due to NDA this is effectively what I'm working with.
JM

 

[ctopher]

The link does not work for me.
How can you turn a turbine blade on a lathe?

Chris
SolidWorks 09 SP4.1
ctopher's home
SolidWorks Legion

 

[SBaugh]

Link is dead - My suggestion to get a 2D profile is to use Intersection curve. I use that often when I need a 2D profile. You can select ap lane that cuts down through the model and select the face and it should convert that.... check the help for clarification.

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

"If it's not broke, Don't fix it!"

faq731-376

 

[TheTick]

If you can determine what the outer silhouette through revolution is, you can create the revolve using a sweep. Make a sweep of a circle with the main path curve being a straight line down the axis. Attach the circle to the silhouette using a point and a pierce constraint. You can then generate a solid that represents the area occupied by the revolution of your shape.

I've used this technique on a couple of occasions. The tricky part is determining your "silhouette", as it is the silhouetted through a curved path, not a straighy projection.

Honesty may be the best policy, but insanity is a better defense.

http://www.EsoxRepublic.com

-SolidWorks API VB programming help

 

[Manifolddesigner]

I agree w/ all your suggestions, but none are ideal.
Due to the nature of the turbine blade, the best I've been able to do is to use the "spline on a surface" command. Then I create several lines adjacent to the surface and along X that terminate with the points of the spline.
This is the best I've been able to come up w/. Then sweep, surface loft, etc.

I know that you can't make a turbine on a lathe, but you can rough the shape out before 5 axis milling. As long as they leave enough material, it'll be fine. I would just like to get it 'right' so we don't ruin an expensive blank and waste a bunch of 5 axis mill time.
MasterCAM actually has this feature built into it, but the fact that MasterCAM's archaic CAD system can do something that solidwork's can't is really frustrating.

JM

 

[kellnerp]

Get the profile using a drawing?

Just my 2cents. Make sure to turn up the curve accuracy in IMage Quality.

TOP
CSWP, BSSE

http://www.engtran.com

http://www.niswug.org

"Node news is good news."

 

[rstupplebeen]

I would create a circular pattern of the blade with whatever resolution you need merging the results. Then I would do an intersection curve and offset this geometry to make a material safe condition. I hope this helps.

Rob Stupplebeen

 

[Manifolddesigner]

rstupple-I thought about that. But it seems really awkward to do like 1000+ body pattern over 10deg and still wouldn't give smooth geometry. I guess the simple answer is solidworks can't do (cleanly) what I want. That sucks.
jm

 

[rstupplebeen]

First, why does the roughing need to be smooth? I was thinking after the intersection you do a fit spline and then an offset.

Second, was the shape of the blade mathematically driven? If so you may be able to create an equation driven curve of the high and low points of the blade and revolve those.

I hope this helps.

Rob Stupplebeen

 

[Manifolddesigner]

It doesn't NEED to be perfect. But it just can't be too wrong. ex, if I leave 0.005" material, but my spline is off by 0.0053"...that would be bad.
It's also extremely time consuming and solidworks is thoroughly unhappy about it. Even with the image settings set nearly all the way up the lines and points and surfaces can be annoying and won't immediately select or will declare that it is overdefined even when it isn't. It really just wants to fight me. (I have legit workstation and video card)

There just needs to be a new feature for this.

 

[BStoner]

Assuming you know the center line you could creating multiple planes along the part. At each place create a circle with the center point along the axis. Have the circle constrained to the outer most part in that section. Create a point to the top of each circle. Then you can create a spline through these points. Next use this spline to create a revolved cut. If the cut fails don't worry it means that the cut does not intersect the part. If it does intersect the part you can highlight these areas and make appropriate changes to the spline.

Brad Stoner
Engineer/Product Development
Legacy Manufacturing

SWx 2006x64 sp4.0

 

[TheTick]

You do not need to make a circular array of densely-packed instances. Take a single piece, and sketch sections normal to the axis of revolution (Tools --> Sketch Tools --> Instersection Curve). Sketch a circle centered on the axis of revolution and tangent to the point furthes from the axis. Do this as needed until your envelope is defined.

 

[Manifolddesigner]

Tick:
You said it: "The tricky part is determining your "silhouette", as it is the silhouetted through a curved path, not a straighy projection. "

I actually tried this first (see spline on surface )
This worked reasonably well until there was a transition from one surface to the next, then it would just fight me and give me overdefined errors and just suck in general.

btw, creating a circ pattern ended up working pretty well. Only about 130 parts over 15 deg. Chopped it up. Saved it as a part, merged bodies and got it.

Still, none of this is "clean" and all are way more time consuming then they need to be. Still needs to be a feature.

JM