Non-rigid body simulation

[anbowden]

Does Algor have the ability to simulate dropping a non-rigid body(e.g. rope or string) onto a fixed, rigid object?  If so, can someone give me some pointers?

Thanks,

Andy

[S.LI]

Hi, Andy,

1.) Most of Algor models are simulating non-rigid body;

2.) To drop something, I recommend MES analysis type;

3.) For your example, One way is that two parts are needed, one for the base (rigid object), another for the rope/string. And the surface contact has to be generated between these two parts. For the base, you have lots of choices, such as brick/tet, or maybe even shell, beam elements. For rope/string, I'm not very sure, maybe you can try truss elements with a small length for each element to simulate a smooth rope.

4.) Another way is to have only one part for the rope/string, and use impact plane to simulate the rigid base. Then surface contact is not necessary here.

[zhuangs]

You can use "MES with Nonlinear Material Models" analysis type.

For the non-rigid body (rope or string), since it is very soft, when you use those line elements, fine mesh will be better, and the modulous will be very small.

For the fixed, rigid object, you can use 3-D kinematic element (for 3D model) or 2-D kinematic element (for 2D model).

For the drop test simulation, there are two ways: surface contact or impact plane.  We (no matter Developers or Application Engineers) usually recommend surface contact be used for drop test analysis now, since:

   (1) surface contact shows better convergence for almost all drop test model;

   (2) surface contact provides more options for the user to adjust the performance.

Of course, current impact plane might work for some drop test models, but it is limited by

   (1) Non-competitive convergence compared with surface contact, for most cases;

   (2) Being perpendicular to global axes.

   (3) Only for flat surfaces.

Hopefully, we will have improved impact plane available in the future.

To use suface contact to simulate your model, you have to define contact pairs in MES contact.  To define contact pairs, you can go to "Help" to find

Help > Autodesk Simulation > Mesh Models > Mesh Overview > Contact Pairs

or use the following link if you are using v2012.

mk:@MSITStore:C:\Program%20Files\Autodesk\Algor%20​Simulation%202012\Help\enu\AlgorHelp_2012.chm::/GU​ID-204E8670-E7B9-439E-B0E2-C6D674A49AC-238.htm

Shoubing 

[anbowden]

Thanks for the replies, guys.  I have a couple more questions, and they might be "dumb questions".

1. When I go to make the contact pairs, it says, "Automatic contact creation did not create any ne contact pairs."  As an alternative, I've assigned general surface-to-surface contact.  Is that OK?  The fact that it won't make automatic contact pairs worries me.

2. What's the best way to simulate gravity?  I assume assign a remote load the rope that only acts in the z-axis.

Thanks,

Andy

[zhuangs]

Hi Andy,

How is your definition of the rope and the rigid object?  For example, your have two parts: part 1 - the rope, part 2 - the rigid object.  In general surfact-to-surface contact dialog, input part 2 as 1st and part 1 as 2nd.  If you know exactly which surfaces have contact, then select the exact surface ID, otherwise, leave "All" there.  If the rope part is using truss or beam element, this part can only be set as the 2nd general surfact-to-surface contact dialog.

One more thing, uncheck the "Adaptive contact stiffness" option.

For gravity, you can easily click "set for standard gravity" in "Setup->Parameters->Gravity/Acceleration", and then input a value of (-1 or 1, depending on the direction of gravity) on Z-multiplier, and 0 for X-multiplier and Y-multiplier.  Note that a load curve is needed for gravity.  And for drop test analysis, this load curve is better set up as (0,1) -> (total time, 1).

Shoubing

[anbowden]

Thanks for the great reply, especially on the weekend!  I have set up the contact surface as you've suggested.  I've set up gravity as you've suggested.

When I have part 1(the big flat contact surface in my case) and part 2(the string in my case) set up as "brick" element types, it will begin to analyze the simulation, but eventually will get hung up at 0.1s.  When I have part 2, the string, set up as "truss" element type, it won't compute and returns an "error due to geometry problem".  Do you have any suggestions how to resolve this issue?  Perhaps my parameters in the truss definition are incorrect?

Thanks,

Andy

[anbowden]

...the error due to geometry problem is, "In working on FEM file or outputting ESH file   Terminal Error: FEM2ESH#59, FEMAPI#2    FEM_ERROR_NO_1D_ELEMENT "

Is it okay to have one part as "brick" and one part as "truss"?  Everytime I Compute Mesh, they both automatically change to "brick" elements.

Thanks again,

Andy

[zhuangs]

How did you create the geometry of the model?  Is it from CAD file?  The truss element is line element.  How did you create these truss elements?  It seems that you meshed the model and then change the element type of the rope to "Truss element".  In this case, there will be error. 

One more thing, for the rigid object, if it is very stiff, it can be set as "3D kinematic element".

Shoubing

[zhuangs]

Hi Andy,

For the case using "truss" element, there might be an error related to generation of truss element.  As you mentioned,

"When I have part 1(the big flat contact surface in my case) and part 2(the string in my case) set up as "brick" element types, it will begin to analyze the simulation, but eventually will get hung up at 0.1s.  When I have part 2, the string, set up as "truss" element type".

It seems that you meshed the model (part 1 and part 2) with brick element. And later you just changed the element type of Part 2 (the string) to "Truss element".  Is my guess right?  If you did like this, this is the reason of "error due to geometry problem".  Since the "Truss" element is line element.

Now let's figure out why "When I have part 1(the big flat contact surface in my case) and part 2(the string in my case) set up as "brick" element types, it will begin to analyze the simulation, but eventually will get hung up at 0.1s."  My questions are:

(1) Does contact start when the model gets hung up at 0.1s? What's the phenomenion in log file,many iterations in each step, high-level of time step, or no change in log file?

(2) How is the mesh size (brick element) in of the rope, especially in the section?  I would recommend the mesh size is very fine?

(3) What is your material model of the rope?

(4) How did you define the contact pair and contact settings? Were you using default?

Please attach a figure of the model and a figure of copying the contact dialog for further information.

Shoubing

---

anbowden wrote:

Thanks for the great reply, especially on the weekend!  I have set up the contact surface as you've suggested.  I've set up gravity as you've suggested.

When I have part 1(the big flat contact surface in my case) and part 2(the string in my case) set up as "brick" element types, it will begin to analyze the simulation, but eventually will get hung up at 0.1s.  When I have part 2, the string, set up as "truss" element type, it won't compute and returns an "error due to geometry problem".  Do you have any suggestions how to resolve this issue?  Perhaps my parameters in the truss definition are incorrect?

Thanks,

Andy

---

[anbowden]

I'm using an Autodesk Inventor assembly file as the basis for the model.  Part 1 is a steel (defined in iProperties in Inventor) slab.  Part 2 is a 1" diameter copper (defined in iProperties in Inventor) helix.  I chose copper because I expected it to be flexible.  I'd like to use a much smaller diameter, but it's difficult to see in the assembly.  Because I used a 1" diameter copper helix, I increased the effect of gravity 100x.  Perhaps that's a poor decision?

Your guess is right.  I meshed the model and then went back and changed part 2("the string") to truss.  Because it's 3D, I suppose the truss model is a bad choice.

(1) Does contact start when the model gets hung up at 0.1s? What's the phenomenion in log file,many iterations in each step, high-level of time step, or no change in log file?

I think the contact begins at 0.05s.  I'm sorry, the log file is a little over my head.

(2) How is the mesh size (brick element) in of the rope, especially in the section?  I would recommend the mesh size is very fine?

The rope is the finest mesh possible.

(3) What is your material model of the rope?

I'm using copper.  You should be able to see the material properties in the attached report.

(4) How did you define the contact pair and contact settings? Were you using default?

I'm using a general surface to surface contact pair.  The default bonded contact setting is the upper level of the tree.  I think you can see this in the screenshot "Initial.jpg".

Thanks,

Andy

[zhuangs]

If you want to use truss element, you can recreate a part for the string in Autodesk Simulation.  If you can a curve line as what you created in Autodesk Inventor in Autodesk Simulation and then divide it into lots of small lines difined as truss element. 

Shoubing 

[zhuangs]

I am a little confused why you increased the effect of gravity 100x.

Now let's focus on the contact analysis. Considering you are using V2011, let's do like this way:
(1) In FEA Editor, right click the workspace and select "General Surface-to-Surface Contact..." to open "Analysis Parameters - MES: Surface to Surface Contact" dialog;

(2) Check whether the contact updating is "Automatic".  If not, change to "Automatic";

(3) Click the value of "Custom" or "Default" in "Parameters" for contact pair 1 to open the "Analysis Parameters - Controls and Parameters for Contact Pair" dialog;

(4) Click "Advanced" to open the "Analysis Parameters - Advanced Controls and Parameters for Contact Pair" dialog;

(5) Uncheck "User adaptive contact stiffness method" if it was checked.

(6) Check "User-defined contact stiffness" and then input a small value of 1000 or some other close values.

(7) Rerun the analysis.

Shoubing

[anbowden]

Hi Shoubing, thanks for getting back to me.

If a 0.035" diameter wire would be easily visible, I would not need to increase gravity 100x.  I'm using a 1" diameter wire and 100x gravity because the 1" diameter is easily visible and I need the wire to fall to the ground as if it were narrow diameter.

For a truss element, I draw a line and then select truss element and add cross-sectional area.  This works fine, but the program won't allow me to run the analysis for some reason.

Contact updating was Automatic by default.

User adaptive contact stiffness was unchecked by default.

The default user defined contact stiffness was approx. 10000 lbf/in.

Here are some things I've been considering:

1. The base should be Isotropic, right?  Should midside nodes be included?  Should it be small or large displacement?

2. The string should be isotropic, right?  Should midside nodes be included?  It should be large displacement, right?

By the way, how long should these simluations take to run?  Mine take approximately 12 hours.

Thanks,

Andy

[zhuangs]

If you just enlarge the diameter of the string and do not change of shape dimesion of the string.  They are different problems.

For MES contact models or other drop test models, I would recommend "Large displacement" be used if there is the option.

Currently, fine mesh is better than coarse with midside node for MES contact models.

For the base, you don't need so much elements, much coarse mesh is fine.  And 3D kinematic element is recommend.

The material model (isotropic or others) is realy dependent on the material and the deformation. Isotropic should work the strain is small, but some other plastic material models should also work if  Isotropic works.

The CPU time is case by case.

When you are using truss element, did you divide the line into lots of elements?

Shoubing