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Thread: Modeling a Nose Gear Fork

  1. #1

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    Modeling a Nose Gear Fork

    Looking for some help to model the abstract form of the legs on a cast fork which supports the nose gear wheel assembly (see picture). The legs curve and twist in different directions. I am not sure where to begin to build this element. Help is much appreciated!

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  2. #2
    SOLIDWORKS Support Volunteer Jeffrey Meyer's Avatar
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    Hi RCS,

    The only tricky part of this geometry is the "3D" C-shaped part, but you should be able to make it with a so-called lofted boss.
    You only need two profiles - one at the root and one smaller one at the "bottom". The bottom one should be on a plane that is at right-angles to the root profile.
    Also, set the end conditions to "normal to the profile".

    Here is a sample:






    Jeffrey
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    Last edited by Jeffrey Meyer; 02-15-2018 at 03:57 PM. Reason: Added images

  3. #3

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    Jeffrey, this is absolutely great help... thank you! A follow-on question if you have time: referring to your images above, it looks like there are several intermediate "sketch stations" (for lack of a better term) which allow the model to be constructed at a granular level of detail. For example in my case the cross section does not change gradually or in a linear manner. Perhaps I want to twist or turn the feature in more complex ways. How do I add this level of detail along the path?

  4. #4
    SOLIDWORKS Support Volunteer Jeffrey Meyer's Avatar
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    Hi RCS,

    The intermediate profile sections that you see in my illustration are generated automatically by the software and presented in the preview. I used only the start and end profiles and allowed the software to interpolate between them.
    However, you have complete control over the path and intermediate profiles - you can define as many as you want by defining intermediate planes and sketching your profiles on them. There are a few pitfalls in doing this (maybe "pitfalls" is too strong a word, let's call them "cautionary steps"):

    1. I strongly recommend that in your loft you use as few profiles as possible. I used only 2 and received pretty cool geometry. I would go as far as to say that 4 of 5 profiles make a very complex loft. This is not to say that you can't use more profiles, but then you have to be very careful with guide curves and start and end tangencies etc.
    2. Try to keep the number of segments constant in each profile. For example, If the first profile is a rectangle with filleted corners (8 segments), and the last profile is a circle, then "split" the circle into 8 circular arcs. Also keep the tangencies between the segments constant.
    3. Try to keep the spacing between the profiles fairly constant. For example, if you use one intermediary profile and place it only 5% (I'm exaggerating to illustrate the point) of the total distance between the first and last profile, I promise you that your loft will not come out very nicely.
    4. Assuming that this is not an academic exercise, make your loft manufacturable: For example, your LG fork will probably be made from a casting in a mold, so start with the mold parting lines as guide curves. and set your profiles to fit between the guide curves. This is an iterative design process: Set parting lines --> define profiles --> loft --> check fit/smoothness/strength/aesthetics/function --> adjust parting lines --> etc.
    5. Lofting is an art: Learn the basics in the SolidWorks Tutorials - "Lofts". Closely related subject: Splines (2D and 3D).

    Hope this helps.

    Jeffrey

  5. #5

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    Jeffrey, your advice is golden and the instructions are very clear. As with most things, practice is the key. I will be putting your instructions to good use and will keep you posted on my outcome. Probably will have some more inquiries as I work on other components. Your feedback is sincerely appreciated! --Rob

  6. #6
    SOLIDWORKS Support Volunteer Jeffrey Meyer's Avatar
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    Hi Rob,
    Glad I could help - also nice to know you have a more human-sounding name than RCS

    Jeffrey

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