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mirroring a 3D spline in 2005 and/or making a sweep with the spline

mirroring a 3D spline in 2005 and/or making a sweep with the spline

mirroring a 3D spline in 2005 and/or making a sweep with the spline

(OP)
I'm relatively new using solidworks and having a real difficult time understanding how to use splines and swept bosses.  Hopefully someone can help me or can point me in the direction to download a simple example.

I'm trying to make a part, it looks, and I just thought of this, and it does, like butterfly wings.  Where you have a spline that shapes the wings, and where the butterfly body is, it's straight.  A 2D spline is all curves, and I can't draw by hand, the 2 wings identical.  If I could that would solve the problem.  I can't draw one wing, mirror it, because I want a sharp edge to mirror about.  

In a 3D spline I can make a spline ending at a endpoint, and can make half the way I want.  But you can't mirror in 3D as far as I can tell.  So for the last 10+ hours I have been trying to make a sweep of the spline, and unsuccessful, and I have been unsuccessful with the example in solidworks because it says I need a pierce point.  I was thinking the sweep would work because, when I tried to make a pyramid before, I found it easy to extrude, make some planes, and make cuts to shape it.  That worked fine, and was thinking, if I could sweep the wing, I can then make cuts to flatten it out to the thickness I need.

So the closest I got, was getting a error needing pierce points, another attempt I made that I thought would work, was with no guide curve.  I closed the 3D spline with a line, then used that as a profile, I drew a circle to use as a path, and got a error "The section profile for sweep is self-intersecting."

Anyone know how to make a butterfly type wings, and extrude it?  This is driving me insane.  I searched on this site, found a thread that was similar, where the person had a problem with pierce points, and tried all the tips that were given there, but none worked.  Maybe I'm missing where the points should go.  

Please help!!!!  I'm determined to sit here until I get this to work!  Please shorten the time!

Thanks very much,
Dan

RE: mirroring a 3D spline in 2005 and/or making a sweep with the spline

Dan,

If you can fit this in a planar (2D) sketch, do so.  Sketch your spline path first.

Next, select an endpoint of the spline and CTRL-select the spline itself and add a plane "normal to curve".

On the new plane, sketch your circle (or whatever your profile is).  Don't pin the sketch to your spline path at this point--just get the sketch to be stable in relation to itself.  If it's a circle, give it a diameter dimension.  Other profiles can be a tad more complex, but the same principles apply.

Select the center of your circle (assuming you want to sweep the center along your path).  Select the spline path.  Select the Pierce relationship and your circle will snap to the path.

Exit the sketch, make sure it's highlighted, and select the sweep feature.  Fill in the pink box for your path by selecting your spline path.  Click OK and you have half of your butterfly.

Select a plane about which to mirror your swept body.  Select the mirror feature.  In this feature, you can select "mirror body", which is what you want.  If possible, select the body from the Solid Bodies folder in the feature manager.  It should mirror the body about the plane you selected.

Create the simpler "body" of the butterfly after your mirror operation.

Hint:  Make your sketched spline path to the right or left of an existing plane in your model--then select one of those planes as your mirror plane--no use making extra work for yourself.

If you get lost along the way, look up the various terms I used in the Help files--everything should work as I've stated.

Good luck.


Jeff Mowry
www.industrialdesignhaus.com
Reality is no respecter of good intentions.

RE: mirroring a 3D spline in 2005 and/or making a sweep with the spline

It's not pretty, but this works...

Make a swept surface using your 3D spline as a guide, then mirror the surface.  You need a section attachet to your 3D guide.  Do it like this:
  1. Make a plane normal to the spline at the spline endpoint (select point and curve for references).
  2. Make a 2D sktch of a short line on the new plane.  constrain one endpoint of the line to the 3D spline using pierce constraint.  Pierce constraint is an option when you select a point on a sketch and a 3D line that intersects the sketch plane.
  3. Close the sketch
  4. Make a sweep surface using the 3D line as a guide and the 2D sketch as a section.
  5. Mirror the resulting surface body, and you can use the edges as references for other features.
Is your part not symmetrical?  It sounds to me like you could model half and then mirror.  Sounds like you have a bit to learn.  Wish I could dive in and help.

I could be the world's greatest underachiever, if I could just learn to apply myself.
http://www.EsoxRepublic.com-SolidWorks API VB programming help

RE: mirroring a 3D spline in 2005 and/or making a sweep with the spline

(OP)
Thanks very much!  I just got it to work!  Amazing, once you understand how to do something, it's real easy to do.  Now I fully understand exactly what a pierce constraint is.  I didn't quite follow its meaning in the help.

Now on to the next attempt.  I have this wing, and I want to make a new one, slightly bigger.  radiate doesn't exactly work, so guess a new plane at some angle to radiate out to.  Think it needs a plane to help stretch it.

Hopefully I'll get this one.

Thanks again! That was a lot of help!

RE: mirroring a 3D spline in 2005 and/or making a sweep with the spline

Take a look at Configurations. They are great for making different sizes of similarly shaped parts.


Helpful SW websites every user should be aware of FAQ559-520
How to get answers to your SW questions  FAQ559-1091

RE: mirroring a 3D spline in 2005 and/or making a sweep with the spline

The way I usually mirror 3d spline data is to make a surface from the 3d spline, doesn't matter what kind, as long as the spline becomes an edge on the surface.  You can extrude a 3D spline, which seems a bit odd, but it works.

After making the surface, just mirror it, and now the edge you want is there.

It's a definite kludge, but until SW adds the ability to mirror curves and 3D sketches, this is one way to accomplish it.

Matt

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