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  1. #21
    Forum Deity shift1313's Avatar
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    Just one little thing. You keep saying sketching in 3d planes. There are very few cases when you need to do that. If you right click the mouse you will see new 3d sketch on plane, but if you go up to the new 2d sketch button, below it is a drop down for 3d sketch. These are different.

    Also you should be able to fully define that helmet without having to do any 3d sketches if you plan out all your 2d sketches. It is much easier to define spline curves in 2d rather than 3d so I recommend staying away from 3d sketches unless you have to.

    The same guy i wrote that/those tutorials for asked me about complex surfaces. I still need to make a few more tutorials so if i get the time I will have a few more.
    Matt - Certified Solidworks Expert -Advanced Surfacing, Mold Tool and Sheet Metal Specialist
    Current Software: SolidWorks11,SolidCam11
    http://www.solidworkslessons.info/
    www.mysolidbox.com

  2. #22
    Junior Member Uriah509's Avatar
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    You're a great teacher Matt, you should work for SolidWorks writing tutorials, and they should pay you mad money to do it!
    I was getting very frusterated, and I started re-reading what you have told me and suddenly after repeated trial and error started having absolute success, and understand what was occuring within the relations. Mainly it was the Wrap that was messing me up.

    Using the Offset Entities I figured out a way to even bring out the edge I was having problems with on the goggle Wrap Feature. Got it onto a 2d plane, and it is still fully defined, and seperated from the goggles as its own sketch!

    Rev A Offset front view 2.jpg

    I started a 3d sketch, and holding shift selected the 3d profile ( of the goggles, then applied the offset at 0.9in, and since I was doing this in the front view, as you said, it plotted onto a 2d plane. Works perfectly how I planned it, now the upper midpoint of my new offset profile is level with the construction line relating it to my right view profile for the 'brow'.

    So, to record what I did to get this:

    1) I need to use a 2D profile to wrap which is much wider than the goggles. When wrapped this profile was tailored to fit the way I needed. It stayed fully defined when I wrapped it to the extruded surface representing the 'top down' curvature. Under the surfaces tab I used Delete Face to delete the rest of the extruded surface around the 3D goggle surface. (Note I did a reverse thicken on the lens, maintianing my surface as the exterior one, the backface is just ignored...)

    2) I selected the tangency 'loop' of the 3d profile all at once and converted the entities so then I had the original wrap and a sketch of the 3d profile. When I went into 3d sketch and double click this new sketch, the lines are still black, and fully defined!

    3) I then applied the Offset surface, got the 2D profile with a 0.9 offset, still fully defined! I can now do a reverse offset at the same distance as before to create a new sketch of the wrap profile in 2D.

    Note: Visible in these screens is the original 2D profile I used for the goggles in blue.
    Rev A Offset front view.jpg
    Rev A Offset.jpg

    So that is how to get a spline out of a wrap! Mission accomplished!

    Getting everything else fully defined tonight, and surfaced tomarrow!

    ~"Because if you don't make it, its your own damn vault!".... .. .

    - Best regards,
    Uriah

  3. #23
    Forum Deity shift1313's Avatar
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    Wow thats great uriah! Im glad its working out for you.

    I do still think you should not use the wrap function. It sounds like you are using wrap to make a solid, then deleting the back face(surface). Do you need the lens to be solid at this point in time? Since you extruded that arc as a surface, you could also use the split(under the curves drop down), then delete face. This method would delete the extraneous part of your surface). You could also trim your surface with the 2d goggle sketch.

    Unless I am still not understanding what you need with the goggle I would make your 2 sketches(like you already have), use the projected curve, fill command(with any guides you need for lens shape). From there you can offset the surface(as you did) and you will have your outer and inner lens. At a later point you can loft between the two and knit them together to make a solid(just as I did with the revolved surface near the end of the tutorial).

    There are many different ways to achieve the same end result and there is nothing wrong as long as you get there. The benefits of other methods are usually in time saving(read efficiency), simplicity of the feature tree, and memory. The memory may not seem like an issue but when you get several complex surfaces in a model, every little bit helps!

    Some time this morning I will still try and put a few screen shots up that show pierce and coincident constraints between 2d sketches and 3d curves.

    great work so far uriah!
    Matt - Certified Solidworks Expert -Advanced Surfacing, Mold Tool and Sheet Metal Specialist
    Current Software: SolidWorks11,SolidCam11
    http://www.solidworkslessons.info/
    www.mysolidbox.com

  4. #24
    Forum Deity shift1313's Avatar
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    Here are a few screen shots for you Uriah. The first 3 images were drawn on the standard planes(top, right, front). The 4th image was created on an offset work plane. This is where the pierce relation came in. The 5th is just a loft created with those curves. The last image shows a 3d curve. What i did for explanation was convert that back onto the 2d sketch plane(as a construction line). I applied a coincident constraint between the end points, then a tangent between the splines. So even though the dashed line wont be added to your sketch, this is how SWx uses the tangent relation when dealing with 2d vs 3d curves.
    Attached Images
    Matt - Certified Solidworks Expert -Advanced Surfacing, Mold Tool and Sheet Metal Specialist
    Current Software: SolidWorks11,SolidCam11
    http://www.solidworkslessons.info/
    www.mysolidbox.com

  5. #25
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    Hello, I have a one project regarding helmet. but I have a to make headform using different plane with different angel, I drew all plane and with the origin have some dimension like 0, 20, 40, 60, 70, 80, 90 and 100 after that i joint all point with spline and now, I have bunch of spline in different angel so, I need to joint all together and wanna make surface or solid. How can I do that in SolidWorks. ?Helmet_Arc_11.jpg

  6. #26
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    Registered forum members do not see this ad.

    hi shifty1313. i have tried to view your tutorial but would open a new window and say Not Found. do you have any suggestions to solve this?

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