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  1. #1
    Junior Member Uriah509's Avatar
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    Default Modeling a Helmet using Fully-Defined Lofted Surfaces

    10 Helmet v3.3 Jan 7 201022.jpg

    I am taking an old project out of 3D Studio, and using 3d poly curves as reference lines to draw new splines.

    To maintain that my new splines stay Fully Defined in SolidWorks, I need to sketch each curve from its respective view in 2D, then I need to conform that shape to a 3d surface, representing the third dimension of the curve.

    For instance I drew the goggle lens profile in the front view, and in the top view I drew a 148.5degree arc defining the curve of the goggles. I simply connected the two points of the arc and extruded it vertically up and down so I have a big surface to either wrap or extrude to. This is where I NEED SOME HELP.

    Either way, wrap or extrusion, I just need the spline where the goggle profile intersects the arc extrusion. How do I extract a curve and keep it fully defined without its parent geometry?

    Is there a simpler way I can conform a 2d spline to another 2d spline in an adjacent axis?

    -------------------------------------------------------

    Here is a screen from my project where I used the wrap feature. The 2D goggle profile used to wrap over the green extrusion can be seen in light blue with hidden lines. The poly curve imported from 3ds is the thin yellow 3D goggle profile which I am trying to match. The bright red profile is 3D result scribed to the surface. I just need to widen the 2D profile and mess with it until the wrap comes out the way I need it. Then extract the red profile and do the same process with all the other dark blue and dark red poly curves. Once I get all these done, I can add some splines to further define the surface, and then create a lofted surface.

    new example.jpg


    Thanks in advance for any help!

    Best regards,
    -Uriah

  2. #2
    Junior Member Uriah509's Avatar
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    Default

    PS. It is interesting to note, the Wrap Feature is very handy if I were to manufacture the goggle lens out of Plexiglass or Polycarbonate the 2D profile would be cut out of the required sheet and using heat draped over a surface just like I am using. So in all reality the wrap feature just happens to work perfect for this!

  3. #3
    Junior Member Uriah509's Avatar
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    So how do I extract the blue highlighted 3d profile?

    It seems the parent/child relationship prevents me from getting the profile on its own, without the rest of the extrusion... any ideas?

    new example 2.jpg

  4. #4
    Forum Deity shift1313's Avatar
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    In reality is that lens really flat or is it a bubble shape?

    If you are working with surfaces you can simple use the edge of your goggle in your loft or filled surface. If you simply want that edge you can start a 3d sketch, select the edge and choose "convert entity". This will give you that 3d edge as a sketch line which is "linked" to your goggle.

    For a project like this i would only model one half of the helmet. You will only complicate things by trying to model the whole thing. Just ensure that your have tangency for your spline curves.

    The "curves" drop down on your features and surfaces tab has a Projected curves feature that will let you project a sketch to a surface or a sketch to a sketch. This takes a sketch(say on your top view) and projects it straight up, at the same time it projects a sketch(say on your right view) straight over. The resulting curves is defined by the points at which those two curves meet. This is a handy tool when trying to create 3d shapes while using 2d views. I probably would have done this for the goggle lens as well. A lot of times goggle lenses are flat when produced and the curve is formed by the lens being retained in the goggle(where wrap does come in handy). Lenses that are "bubble" shaped will need some sort of form though.
    Matt - Certified Solidworks Expert -Advanced Surfacing, Mold Tool and Sheet Metal Specialist
    Current Software: SolidWorks11,SolidCam11
    http://www.solidworkslessons.info/
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  5. #5
    Junior Member Uriah509's Avatar
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    Thank you so so much for all that great information and suggestions! Couldn't have asked for more.

    Yes, the lens does have curvature, but I don't have enough information to define it anytime soon. I will have to do a physical mach up of the helmet so I can check Field of View, and optical distortion of the lens.

    Thanks again!

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    Forum Deity shift1313's Avatar
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    no problem Good luck with the project and dont hesitate to ask any more questions along the way.
    Matt - Certified Solidworks Expert -Advanced Surfacing, Mold Tool and Sheet Metal Specialist
    Current Software: SolidWorks11,SolidCam11
    http://www.solidworkslessons.info/
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  7. #7
    Junior Member Uriah509's Avatar
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    So I did the sketching with 3d planes tutorial twice, but I can't seem to be able to convert the wrapped edge/profile.

    I get the error "Convert Entities - Only curves and points from this sketch can be projected onto a 3D sketch plane"

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    Forum Deity shift1313's Avatar
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    You are having issues converting the edge of the goggle lens? I dont supposed you could you could upload the part could you?
    Matt - Certified Solidworks Expert -Advanced Surfacing, Mold Tool and Sheet Metal Specialist
    Current Software: SolidWorks11,SolidCam11
    http://www.solidworkslessons.info/
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  9. #9
    Forum Deity shift1313's Avatar
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    I was thinking about this earlier today and i wanted to mention to you several other ways to create your goggle shape. Firstly you do not need to create the solid or any parts for that matter. If you were simply going to create the 3d curve for the lens you can simply draw your top down view of the goggle arc, then the front view of the goggles. From there you do a Projected Curve, select Sketch on Sketch and select your two sketches. This will give you the 3d curve.

    With that if you like you can do a Fill Surface for the 3d curve. This will give you a nice surface to work with. If you want a solid, you can use the Thicken command.


    If you want to work with 3d curves this is probably the quickest and most efficient method. You could also work with surfaces and their intersections, surfaces cutting solids, Surfaces as start/end points for extrusions and as you used Wrap.

    There is also the technique of creating a Die and forming the goggle by creating a flat part. This is used for sheet metal parts but could technically be applied here.

    If i were to draw this i would use the sketch on sketch projection.
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    Matt - Certified Solidworks Expert -Advanced Surfacing, Mold Tool and Sheet Metal Specialist
    Current Software: SolidWorks11,SolidCam11
    http://www.solidworkslessons.info/
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  10. #10
    Junior Member Uriah509's Avatar
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    Registered forum members do not see this ad.

    Right, I understand the Projected Sketching.

    I really need to use the wrap feature for the goggles as we discussed, but for learning's sake I can skip it for now, ruff up the goggle in a projected sketch and work with the rest of the helmet that way.

    I am learning on SW 2010, I believe 2009 can't read my files.

    In the future I will understand the software enough to be able to extract the 3d profile. I must not be using my planes correctly, or something, as I don't understand the error I am getting.

    Thanks for finding the fill surface and thicken!
    Last edited by Uriah509; 26th Apr 2010 at 08:42 pm. Reason: revision

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