How to design a flexible body in solidworks2011?(I want in study motion after apply force it's stretched)

(I want in study motion after apply force it's stretched)

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5 Answers

I don't think you can do that. Someone will correct me if I'm wrong, but as far as I understand how SW and other similar apps work, the created solids are what the name tells: solids - infinitely rigid bodies. Even if you apply water, air or rubber as material. That changes only when you work in Cosmos/Simulation when the resistance to applied force/pressure varies in dependence of the applied material attribute. Look at spring, automotive tire, bicycle spoke designs... They are all flexible in real life, not so much within the program. The more constraints you add (dimensions, definitions), more inflexible it becomes. Don't apply enough constraints, and it blows apart... :(

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Here is my lengthy comment, I think it's worth its own answer...

You can make the part look like it deforms a bit when lengthening it. You should use sketch relations in a smart way though, but it is possible. Take, for example, the situation I have taken above as well. You have two plates in your assembly: one fixed, one able to go up and down. Now:
-Create a new part inside the assembly: Insert>Create new part
-pick the top surface of the bottom plate as the base reference plane.
-sketch a line on this base reference plane that end in the midpoint of the plate.
-Insert>reference geometry>Plane, and select the drawn line, and the line's end that coincides with the midpoint of the plate.
-go to the sketch tab, then: Sketch>3D Sketch
-now click the bottom surface of the top plate (the plate that can go up and down, but is 'fixed' while making this new part!) and press 'Convert'. This will create a square that is fully related to the edge of the moveable plate.
-Draw a diagonal in this new square, that runs from (for example) the left bottom corner to the right upper corner. Pick the midpoint of this line and use it as a starting point for another line, which has to end in one of the free corners of the square (for example: Left upper corner).
-Open a sketch on the plane you have made before. make sure you look straight at it by right-clicking the plane in the manager design tree, and then click the icon that looks like a plane with an arrow perpendicular to it.
-There are two points that coincide with the plane you have made: the center of the lower plate and the center of the upper plate! Connect them with a straight line.
-Draw a straight line horizontally, with the lower midpoint as starting point. This will be the radius of the 'flexible' column. Define this size!!
-Also draw a straight horizontal line with the upper midpoint as a starting point, in the same direction as the previous line. This will be the radius of the 'flexible' column at the top. Define this size too!!
-Pick the middle of the vertical line (which is your center line now) and draw a horizontal construction line in the same direction of the radius lines, though make sure it does not get related to either the endpoints or midpoints or anything of the radius lines! Set (note: NOT define!) the length of this line manually to the same as the radius lines, so that the 'flexible' column will be straight in the current position of the plates. This line, now, is the stretching radius line. Make sure this line has a ' Perpendicular' relation to the center line!!
-Are you feeling sleepy? Take a strong cup of coffee or other brew, then come back and continue please!
-Draw a construction line from the lower midpoint to the end of the stretching radius line. Also, draw a construction line from the upper midpoint to end of the stretching radius line. just for symmetry...
-Define the length of at least one of these two somewhat diagonal construction lines. DO NOT alter the length, leave it at the current length it has! just define it at this length, so that it won't shorten when you will 'pull' or 'push' on the 'flexible column', and ruin your (so far) great day.
-Now pick the spline tool and click on the end of the upper radius line, the end of the 'stretching' radius line and the end of the lower radius line.
-Leave the sketch, go to the feature tab, pick 'Revolved boss/base', and you are golden! This is the 'flexible column' everyone excluding your closest friends are talking about!

Enjoy, and don't forget to make your own variations! this is just an example of how it could be achieved.

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Robert is correct. You can't flex or stretch anything in SW like you can in real life. There are some programs out there that can do that, but SW just isn't powerful enough because it is more of a design program than an analysis program.

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I agree with the other two answers. There are ways, though, to make things look like they can stretch. For example: make two separate .sldprt flat square plates. Put them both into an assembly. Fix one by mating its front/right/top planes with the assembly's front/right/top planes. Mate the other only in the front and right plane, so it can still move freely in the heigth-direction. Now click on Insert part>New part and click on the top face of the bottom (the fully fixed) plate. Draw a circle, and click on features>extrude. Now find in the drop-down box (that is now saying 'Blind') the option called Up to surface. Select it, and then click the bottom face of the upper (not fully-fixed) plate. It's even better if, when you have drawn the circle, you also draw a line to the middel of your circle. Now Insert>reference Geometry>plane and select the line and the end point of the line that coincides with the circle's mid-point. Now open a sketch on the new plane, draw a (straight) line from the midpoint up to the bottom surface of the upper plate (make sure it 'snaps' to that surface). Make sure to NOT FULLY DEFINE that straight line! If you do, it won't be flexible. Leave the new part and rebuild your assembly.
Now move the upper plate upwards. You see a gap between your new part and the upper plate. Now rebuild your assembly, and the new part will have stretched to reach the bottom surface of the upper plate again.

If that is all too fuzzy, just download any SolidWorks assembly which has a 'working' suspension, like my padlock. But those geometries will only stretch (or shrink) when you rebuild your assembly again! Great for animations though, but I don't guarantee it will fullfill your needs...

I have attached my padlock. Make sure to put the key in the same folder as the other padlock files! Then open the padlock.sldasm and check out how it works.

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