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  1. #1
    Hi
    I am trying to make a crane.I have already made the structure of the crane. The last part is to connect a hook and a rope. i don't know how to make a flexible part in solid works. can anyone help me with that.

    Another problem I am having is when I make assembly using parts and other assemblies the other assemblies do not behave like they do separately. The movement of the parts are not available in the bigger assembly. Is there any way that the smaller assemblies behave same in the big assembly too.

    Thanks

    Tava
    =============
    Tava

  2. #2
    Rope: do you have the SolidWorks Premium license? It contains the SWX Routing add-in which is supposed to be used for wiring and plumbing. I've tried to use it in the past (no training), but gave up in favor of this:
    1. <LI>Make a 3D sketch in your assembly where you want to route the rope- create a spline and constrain it accordingly.</LI>
      <LI>Insert > Component > New Part > pick your template > choose a plane for sketching the rope cross section (you may have to create a plane for this earlier in this process). Sketch the ropeprofile.</LI>
      <LI>Start a 3D sketch, and pick the spline. Click "convert" toolbar button to convert it to a sketch entity in your active sketch.</LI>
      <LI>Using the profile and 3D sketch, sweep your rope.</LI>

    To make a sub-assembly flexible: (from the help files)
    1. <LI =kadov-p>


      Right-click a sub-assembly in the FeatureManager design tree and select Component Properties. The Component Properties dialog box appears.
      <LI =kadov-p>


      Under Solve as, select Flexible, then click OK.
      In the FeatureManager design tree, the icon changes to [img]mk:@MSITStore:C:\Program%20Files\SolidWorks\lang\e nglish\sldworks.chm::/art_otherUI/FM_Icon_sub-assembly_flexible.jpg[/img] to indicate that the sub-assembly is flexible.</LI>

  3. #3
    Hello

    First of all I want to thank you for your detailed solution. I am very happy that I have almost completed the crane assembly. i am using Solidworks Student version.

    i just did what you said but stuck in the middle. I have some questions about the process.

    1. Should I draw the 3D spline in the assembly or should I draw it separately as a part. I tried both. If I draw it in the assembly then I can not use the swept boss feature because there is no such option in assembly (well I can not find it, it may be hidden some where. I searched in the feature button,it was not there).

    2. If I draw it separately as a part, it is like a rod bent in some given shape.When I inserted it in my assembly it doesn't behave like a rope.

    3. What is this "Convert" does. I tried to convert my 3D line but it gives some error message. Is it a necessary step?

    4. I want to add a winch and then wrap the rope in it so that by rotating the winch the hook moves up and down. Is this possible. Please tell me how to do that.

    5.My last question is when I tried to make the assembly flexible in the properties window the SOLVE AS options were grayed so cant change it. Can you tell me a soln.

    I really appreciate your help

    Thank you

    Tava
    =============
    Tava

  4. #4
    To answeryour questions:
    1. <LI>Draw the 3D line for the rope path in the assembly. You then create your part "in context" and sketch the rope profile (cross section). Within this same part, you create a 3D sketch, and effectivly copy (convert) the 3D line in the assembly, so that now you have an exact copy in your part. Now you have an externally referenced path and a profile for your sweep.</LI>
      <LI>This is because the part you created did not have an external reference to the assembly. For something like a rope, external references are unavoidable.</LI>
      <LI>The "convert" command needs to be done editing your rope "in context." You may need to right click the rope part and click "Edit Part" or "Edit Subassembly." Don't forget to click the top assembly level and right click "Edit Assembly" when done. To get to "convert" command: Click Convert Entities [img]mk:@MSITStore:C:\Program%20Files\SolidWorks\lang\e nglish\sldworks.chm::/art_tools/Tool_Convert_Entities_Sketch.gif[/img] on the Sketch toolbar, or click Tools, Sketch Tools, Convert Entities.</LI>
      <LI>It may be possible, but this type of functionality is beyond me. There is some kind of "belts" funcionality- you might try searching the SWX Help for it.</LI>
      <LI>I could not reproduce what you've described- what SWX version are you using? Also, is it Premium or Professional?</LI>

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