Select profile for Extrude?

Discussion in 'SolidWorks' started by SR, Jan 7, 2004.

  1. SR

    SR Guest

    I am using the 2D to 3D toolbar to convert 2D DWG files into 3D
    solids, but have a question about selecting entities to Extrude. It
    appears I have to select each entity in the profile I want to extrude
    and want to know if there is an easier way to either fence select or
    chain select the profile to be extruded? The profiles I am using are
    pretty complex and require that I constantly zoom in and out in order
    to select each segment.
     
    SR, Jan 7, 2004
    #1
  2. Would selecting a region help. It sounds like you may misunderstand the 2d
    to 3d thing. What it is supposed to do is you

    open an AutoCad drawing in SW
    your AutoCad drawing has 2 or 3 views.
    You window select the first view (if you need to use multiple windows to
    select the whole view you have to hold CTRL down when making the next
    selection)
    then once you have selected the first few you hit the button labeled front
    (this moves every selected entity into another sketch.)
    you repeat this for your side view and hit the appropriate side view button.
    the only difference is sw now rotates this sketch 90 degrees so you can
    (cut)-extrude them into each other
    once your views are on the right planes Hit rebuild and select the sketches
    you want to extrude.

    if you are working with simpler parts you can open the part in AutoCad and
    copy the front view and simply paste it into a new part. and extrude.



    Hope this helps

    Corey Scheich
     
    Corey Scheich, Jan 7, 2004
    #2
  3. SR

    SR Guest

    Thanks Corey. I appreciate the reply, but I'm comfortable with
    everything you mentioned (i.e. defining view orientations - Front,
    Top, Right). The problem I have is - quoting your reply "once your
    views are on the right planes Hit rebuild and select the sketches you
    want to extrude." selecting the profile for the extrude. I can do it,
    but it means that I have to go around the profile and select each
    segment one at a time until I have selecting the entire closed
    profile.

    I'm not sure what you mean by a region? but if it reduces the number
    of screen picks I have to do to identify my profile then great! I
    looked in help and didn't see it?

    SR
     
    SR, Jan 9, 2004
    #3
  4. You need to select the sketch first then hit extrude.

    There are 2 extrude commands. One is on the 2d to 3d tool bar the other is
    on the Features tool bar.

    The one on 2d to 3d if you select a line on your sketch and hit this button
    it will move the line you select into another sketch and extrude it. If you
    created your front and side sketches as I explained the lines that you
    selected for them will turn black and you will have a few sketches in the
    design tree to the right.

    Sketch1 (Was origionally your imported drawing)
    Sketch2 (Should be your front sketch)
    Sketch3 (May be your right side sketch)

    If you select sketch2 from the design tree and hit extrude it will extrude
    every line that you put into your front sketch.

    Then you select sketch3 and hit cut-extrude flip side to cut and depending
    on complexity you should have your part.

    If your part is more complex you can cut or extrude by region, it is at the
    bottom of the extrude dialogue.

    The above can be done without hitting rebuild

    If you do hit rebuild after creating Front and Side sketches and use the
    Extrude button on the feature manager you don't have to select from the
    design tree. Now you will be able to select a line that is in your sketch
    and the whole sketch will extrude.

    (this is all assuming that you don't have overlapping regions and that your
    contours are closed. If you have overlapping regions use the regions feature
    of the extrude commands as described above

    Clear as mud?? =)

    Corey
     
    Corey Scheich, Jan 9, 2004
    #4
  5. SR

    SR Guest

    o.k. Your detailed reply has helped me isolate the problem.

    What I was doing was selecting the profile sketch by selecting each
    segment of the profile (not selecting the sketch from the tree). The
    reason I was doing this is because after defining the front, top and
    right sketchs using the 2d to 3D toolbar the planes are automatically
    offset from each. Therefore in order to extrude the profile with an
    offset from the plane it was defined on I was also selecting a point
    on an adjacent profile (for example I would select the front profile
    and closest point on the top sketch as the offset or starting point
    for the extrude). By doing this the extrude would begin offset from
    the sketch plane to where it needs to start. This procedure works find
    except you cannot select the sketch profile in the tree as per your
    directions "and" select a point on another sketch to account for the
    planes offset.

    If you use your method you save time from not having to select each
    sketch profile segment, but do not account for the offset when
    extruding. A subsequent cut-extrude is then done to cut the offset out
    (flip side) followed by additional cuts etc.

    Because my profiles are pretty complex I like your method better, but
    it would be nice to save the cut-extrude side to get around the
    offset. Not sure why they even offset these sketches anyway...

    Something else I learned from you was after defining the front, top
    and right views - turning off sketch1 eliminates a lot of clutter.

    Thanks,
    SR
     
    SR, Jan 12, 2004
    #5
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