AnsweredAssumed Answered

Force/Load vs Displacement on a solid model simulation?

Question asked by Adrian Warga Kane on Jun 20, 2013
Latest reply on Jun 21, 2013 by Jared Conway

Like • Show 0 Likes0
Comment • 19

I'm working on a halved model of a sidewall deflection test. My question is can anyone give me an idea how to get a graph that displays the FORCE vs DISPLACEMENT of the load on my cup? (The load being the pusher that is on top of the halved cup in the tray) I haven't been able to tweak the graph options to find it yet. The best I can do is Stress vs displacement.

I'm going to include the files if you want to play around. I'm using a nonlinear study.

Once again I'trying to graph the force of the load on the cup vs displacement of the load coming down on top of the cup. Any insight?

Adrian

Attachments

setup19jun13 1.5X.SLDASM.zip296.3 KB
.5KC16S (simplified) (1.5X).SLDPRT.zip675.1 KB
.5Pusher.SLDPRT.zip137.4 KB
.5angledtray.SLDPRT.zip119.5 KB

No one else has this question

Outcomes

19 Replies

Brian Zias Jun 20, 2013 4:05 PM
Mark Correct
Correct Answer
Hey Adrian,
I haven't taken a look at your files so I am not sure how you have set up the Pusher force/displacement. I would suggest to set up this problem using an Enforced/Prescribed displacement. Add a Restraint in the normal direction to the top of the Pusher, and in the Fixture Property Manager, add in a value where the vertical (pushing) direction is zero, say 10mm. Notice you can vary this using a curve, but say you just leave that linear. So know you know the displacement vs. "time".

Then, at each solution step, you can RMB on the Results folder and List Result Forces... and then click the face to which you applied the restraint. This will show you how much Force it took to enforce that displacement that you prescribed. If you do this for each step (I forget if this tool will let you plot it over time automatically...) then you will have force vs. "time" and should be ready to compare back to your displacement vs. "time".

Brian
Like • Show 1 Like1
Actions
- Adrian Warga Kane @ Brian Zias on Jun 20, 2013 4:17 PM
  Mark Correct
  Correct Answer
  Hey Brian, I believe I set up a restraint so the pusher can only fall 1 inch max. Is that what you're referring to by "Restraint in the normal direction to the top of the Pusher"?
  
  Also, I'm not quite sure what the fixture manager is.
  Like • Show 0 Likes0
  Actions
  - Brian Zias @ Adrian Warga Kane on Jun 20, 2013 4:22 PM
    Mark Correct
    Correct Answer
    Hey Adrian,
    If you added a 1" value to the Restraint (the Fixture Property Manager is the box that you put in all the settings for the restraint - sorry for the SWX lingo) then you are forcing the pusher to displace exactly 1", not "fall 1" max". So you should see in your results the pusher displacement at exactly 1" at the end of the time range.
    
    Whatever face you applied this restraint to, you can click on and get the Result Force that it took to make that result happen, which should be the force exerted on the cup body (well, half of it in your case).
    
    Brian
    Like • Show 1 Like1
    Actions
    - Adrian Warga Kane @ Brian Zias on Jun 20, 2013 4:28 PM
      Mark Correct
      Correct Answer
      I think this is what you're talking about.
      Like • Show 0 Likes0
      Actions
      - Brian Zias @ Adrian Warga Kane on Jun 20, 2013 4:32 PM
        Mark Correct
        Correct Answer
        Yep this is good. A couple suggestions:
        1) Remove the force on the pusher face. It is redundant if you are also prescribing a displacement. Remember if you tell it to move 0.75", that face will move 0.75" with no force needed, and in fact it is the result force you're trying to determine. So delete that force.
        2) Move that restraint to the flat face (the one showing the pink plane in your image) so it doesn't interfere in the contact surfaces.
        3) make sure you have surface to surface contact in between cup and pusher and a decent mesh.
        Like • Show 0 Likes0
        Actions
        Adrian Warga Kane @ Brian Zias on Jun 20, 2013 4:37 PM
        Mark Correct
        Correct Answer
        Thanks. Is there an easy way to mate it exactly to the surface? In my my mated assembly, I basically inched the pusher down by using a displacement mate which makes for a very rough exact surface mate.
        Like • Show 0 Likes0
        Actions
        Brian Zias @ Adrian Warga Kane on Jun 20, 2013 4:39 PM
        Mark Correct
        Correct Answer
        I would think a Tangent Mate would work here.
        Like • Show 0 Likes0
        Actions
        Adrian Warga Kane @ Brian Zias on Jun 20, 2013 4:42 PM
        Mark Correct
        Correct Answer
        It only allowed me to make a perpendicular mate, not a tangent one, so that's why there's a small offset, I believe.
        
        So when you say move the restaint to the flat surface you're referring to the top of the pusher? so it displaces down from that point say .75 inches?
        Like • Show 0 Likes0
        Actions
        Brian Zias @ Adrian Warga Kane on Jun 20, 2013 4:49 PM
        Mark Correct
        Correct Answer
        Yep the top of the pusher. Keep that 0.75" value in the Vertical/Normal direction, and also enable the other two directions with zero values which will make sure the pusher moves only in that one direction.
        
        Hmm, not sure why tangent doesn't work here between the round face and the cup... a workaround: mate the pusher so it can only move in and out in the pushing direction, then use Move Component with Collision Detection to move the pusher in until it collides, then Fix the part at that position. Dirty but should work. There are other mates that could work, like using a point on path.. but that would be more work.
        
        Brian
        Like • Show 0 Likes0
        Actions
        Adrian Warga Kane @ Brian Zias on Jun 20, 2013 5:00 PM
        Mark Correct
        Correct Answer
        I'm not completely sure this is what you meant but here's what I did.
        
        Also is collison and interference detection the same?
        Like • Show 0 Likes0
        Actions
        Jared Conway @ Adrian Warga Kane on Jun 20, 2013 5:00 PM
        Mark Correct
        Correct Answer
        this should work fine for what you want to do
        it tells the block to move 1 inch downwards but 0 in the other directions
        Like • Show 0 Likes0
        Actions
        Adrian Warga Kane @ Jared Conway on Jun 21, 2013 8:16 AM
        Mark Correct
        Correct Answer
        Thanks, man. I really appreciate the confirmation. As a self taught simulation user, sometimes I'm drowning in my lack of knowledge.
        Like • Show 0 Likes0
        Actions
        Brian Zias @ Adrian Warga Kane on Jun 20, 2013 5:01 PM
        Mark Correct
        Correct Answer
        Looks good! Does it solve? You may have faster solve if you make the cup into a shell mesh. But you can also run a quick Draft-quality solid mesh to make sure the displacement behavior is as expected.
        Like • Show 0 Likes0
        Actions
        Adrian Warga Kane @ Brian Zias on Jun 21, 2013 8:14 AM
        Mark Correct
        Correct Answer
        It sort of solves, it usually gives an error around 60%, but the animation for it doesn't look half bad. I think it's partly due to my low quality mesh.
        
        What do you mean by shell mesh? actually turning my cup into a shell instead?
        
        Also do you think my reference geometry for holding the half cup in place is sound?
        I did this by accident. But it might have still worked. I used the top plane and ,made it move 0 along dir1.
        
        I meant to contrain it to the front plane and normal to to plane but I think both copuld work? II just used a weird relationship on accident it seems.
        
        Also, I really appreciate it, man. You've been incrediably helpful.
        Like • Show 0 Likes0
        Actions
        Jared Conway @ Adrian Warga Kane on Jun 21, 2013 11:14 AM
        Mark Correct
        Correct Answer
        Adrian, it would be helpful if you hid all other BCs to show the ones that you're trying to highlight.
        
        for symmetry, you just need a restraint that is normal to the face
        
        to hold the assembly from sliding in the y direction it looks like you restrained the bottom face, taht should be good
        
        to restraint it in the x direction (Assuming z is the symmetry plane normal), restraining the vertex at the origin in the x directino should be plenty.
        
        for the cup, contact at the leading and trailing edge should keep it in place. just make sure you've created it. if you want to help the solver out or at least while you're starting, you might want to just over restrain it by fixing a point in the center at the back side of the cup in the x direction only.
        
        and solid elements > shell elements, you'll bring down the size of the problem and be able to get better results. with solids you need 2 elements across the thickness to get good stress results. (high quality) draft quality elements for either will give you an idea of the shape of deflection but it will be overly stiff and also won't help with stress results.
        Like • Show 0 Likes0
        Actions
Jared Conway Jun 20, 2013 4:27 PM
Mark Correct
Correct Answer
it's been awhile but i don't think you can do force vs displacement, i think there are a couple of enhancements for this.

since it sounds like you added a displacement restraint (to create a prescribed displacement) your output is force on those faces. you can use the displacement plot for force OR the results force plot to output that information vs time.

then you'll have to combine the information for your displacement (which is linear) and force in excel and you can create force vs displacement.
Like • Show 0 Likes0
Actions
- Adrian Warga Kane @ Jared Conway on Jun 20, 2013 4:45 PM
  Mark Correct
  Correct Answer
  I know there's one way, but I can't get to it. There's a tutorial in SW simulation that shows a load vs distance but that's using a non linear study and arc length properties which I think can only be done with shells.. I was just hoping there was another way.
  
  Snap-through/Snap-back of a cylindrical sheet is the tutorial I believe.
  Like • Show 0 Likes0
  Actions
  - Jared Conway @ Adrian Warga Kane on Jun 21, 2013 12:15 AM
    Mark Correct
    Correct Answer
    adrian, i think what you're describing is 100% specific to the arc length control method. i think the enhancement specifically calls out an output similar to that for other studies.
    Like • Show 0 Likes0
    Actions
    - Adrian Warga Kane @ Jared Conway on Jun 21, 2013 8:16 AM
      Mark Correct
      Correct Answer
      Ah, that's a shame, I was hoping to be able to maybe apply that to this, but I think arc length control mentod only works for shells so I'd have to move in that direction if I wanted to use that way.
      Like • Show 0 Likes0
      Actions

Force/Load vs Displacement on a solid model simulation?

Attachments

Outcomes

Related Content

Recommended Content