setting 'no compression' for truss element, causes abort... modeling ligament as tension only truss 1

[MrSamuel]

I am trying to model a ligament with a truss. To make it somewhat realistic, I need it to be tension only. The only way I have found to do this is to turn on "no compression" for its respective material. This causes my simulation to fail, giving me a bunch of the following errors:
Solver problem. Zero pivot when processing D.O.F. 3 of 18 nodes.

What happens when a truss with no compression is compressed? No reaction force?
Is there a different way to make a truss tension only?
Any suggestions?

Thanks,
Sam

 

[IceBreakerSours]

If you open the ODB in CAE, you will find out where the zero pivot nodes are. If these nodes are on the ligament(s), then, in all probability, you forgot to constrain the rotational degrees of freedom. Keep in mind, trusses are structural elements and nodes on structural elements have 6 degrees of freedom unlike nodes on continuum elements which have 3.

In other words, nodes on the ligaments (i.e., trusses) are free to rotate under an applied load.

~Ice!

http://www.eng-tips.com/faqs.cfm?fid=376

 

[MrSamuel]

I'm trying to look at the zero pivot nodes. I'm using abaqus cae, so I right click on the job and select 'results'. I open up the display group manager but not sure what to do from there to view the zero pivot nodes... any tips?

Though I'm realizing its a moot point, I get the zero pivot error whether or not the simulation finishes successfully (I just realized this now...).
The simulation is successful when I don't use 'no compression', and fails when I do use 'no compression'. The zero point error has nothing to do with it...

Is using 'no compression' the correct way to make a truss tension only? Is there another way?

Thanks for the help so far,
Sam

 

[IceBreakerSours]

You must get rid of zero pivots irrespective of whether the model converges or not. Read the documentation for more on zero pivots/overconstraints.

Coming to the visualization of these zero pivots, I would recommend getting more comfortable with the GUI by going through a few examples. In the Display Group, click on Nodes. In the list of nodes in the panel on the right, there will be a bunch of warning nodes saying something like zero pivot for some degree of freedom at node #.

~Ice!

Additional information:

I have rarely used structural elements so I may not be entirely accurate but using the "no compression" argument sounds right to me. However, sometimes the no tension/compression modified linear elasticity can make the model unstable. I guess this is due to a sharp transition in the stress/strain curve, which must make the tangent stiffness (slope of the stress-strain curve used by the iterative algorithm) non-smooth. In any case, if static analysis is being performed, some artificial stiffness may be added to the model by the stabilize argument in the step definition.

http://www.eng-tips.com/faqs.cfm?fid=376

 

[MrSamuel]

I was able to look at the zero pivot problem nodes. Turns out a couple ligaments weren't attached. So I've fixed that, thanks.

But still the same problem exists. Setting 'no compression' makes the simulation fail. I bet you're right about it resulting in sharp transition in the stress strain curve. There are three different stabilizations I can choose from. I'm trying Dissipated energy fraction first with automatic stabilization turned on. My first attempt with the default numbers didn't fix the problem. I'm really shooting in the dark here, any suggestions what stabilization and numbers to try?

Thank you kindly for all your help so far, Ice


If anyone else is listening in here, is there any other way I might try to simulate a ligament such that it is tension only?

 

[IceBreakerSours]

Default parameters in the stabilize argument in the step definition should be fine. If this is not working, then something else is wrong in your model.

I would think about the following questions: Is this a 2D/3D model? What are the loading/boundary conditions? Are there any warning nodes/elements? What do the .msg/.dat files say? When does the model fail (in the .sta file)?

I imagine you are more interested in joint motion since you are applying linear elasticity to ligaments; as you must know, ligaments are quite nonlinear. Linear elasticity will result in a stiff joint at lower loads/deformations and, perhaps, not so stiff joint at high loads/deformations. If you care about end-state loads/deformations of the joint at moderate loads/deformations, then linear elasticity may work just fine. But if that is not the case, then you should look into hyperelastic (or rubber-like) material models, the simplest one being Neo-Hookean. Google search will get you the material parameters appropriate for ligaments. Ultimately, however, a more advanced model (like Weiss or Holzapfel) will be needed if you are interested in a more accurate model of the ligament.

If you want to explain the goals and scope of the project, perhaps, I could suggest a few things. For example, are you interested in ligaments (fiber stress/strain) themselves or are you more interested in the motion of the joints? Which ligaments are you interested in? I am sure its a 3D application but are you interested in transient or equilibrium state behavior, i.e., dynamic vs. static analysis?

Note that the highlighted keywords are to emphasize the subjective nature of these terms. Your engineering skill will come in to play while defining these terms.

http://www.eng-tips.com/faqs.cfm?fid=376

 

[MrSamuel]

I'm trying to load a foot model onto a flat surface. The foot model consists of bones (rigid), ligaments (elastic), plantar fascia (elastic), and soft tissue (hyperelastic). I think the elastic assumption for ligaments and fascia is OK because I am after joint angles and pressure between the soft tissue and ground.
The tibia, fibula, and soft tissue are fixed at the top (ankle) and the ground is first displaced into the foot to achieve contact, then loaded onto the foot to simulate weight bearing. Force is also applied to the calcaneus as the achilles tendon would normally do during weight bearing.

I was hoping to upload the file for you but it seems 10mb is too big... I'm getting a server error

Just the simple change of making the ligaments tension only causes it to fail part way through the first step (displacing the ground to achieve contact); the increments get smaller and smaller until they are smaller than the minimum or too many attempts have been made.

What is odd is that it runs just fine with no ligaments at all! So you must be right that instability is occurring at the transition from tension to nothing at all... I will try the other two stabilizing methods.

I have some warnings, the same ones whether or not it fails. I don't think any of them are of any consequence (below)

Thanks!
Sam

Whenever a translation (rotation) dof at a node is constrained by a kinematic coupling definition the translation (rotation) dofs for that node cannot be included in any other constraint including mpcs, rigid bodies, etc.

The thickness is considered by default in the tied pair (assembly__pickedsurf1024,assembly_cuboid-1_surf-1). To ignore thickness, specify the 'no thickness' parameter in the definition of *tie.

The ratio of the maximum incremental adjustment to the average characteristic length is 1.08649e-02 at node 3858 instance softtissue-1 on the surface pair (assembly__pickedsurf1024,assembly_cuboid-1_surf-1).

For *tie pair (assembly__pickedsurf1024-assembly_cuboid-1_surf-1), not all the nodes that have been adjusted were printed. Specify *preprint,model=yes for complete printout.

 

[IceBreakerSours]

If you wish, you might be able to upload the CAE file, if not the INP. You could also attach screenshots or a slideshow if you wish.

Some questions for you:

1) Is this a static or a dynamic analysis? Are you using Standard or Explicit?

2) Did datacheck run without any issues?

3) Since the model converges with default linear elastic properties for ligaments, see if any of the ligaments undergoes compression in step 1. If yes, then check if the stabilization energy increases or not (it should) near the end of simulation time in step 1 where the model fails. You can view this by opening up the odb in the Viewer and checking the odb history options.

Also, with default linear elastic properties for ligaments, are there any warnings/signs/messages in any file?

4) What is ground? Is it a rigid surface?

http://www.eng-tips.com/faqs.cfm?fid=376

 

[MrSamuel]

Its a static analysis using standard
I'm not sure what data check is. Is this what goes on until the submission is accepted?
I'm not sure how to check on stabilization energy, I will have to look into this...
Ground is steel for now

The good news is that it worked! Messing around with stability controls I was able to make it get passed the unstable parts. But the whole thing ran a lot slower and is very finicky. Slight changes in loading conditions make it too unstable to complete. I wish it were more robust, but this is a big step.

Thank you for the idea of using stability control!

I would like to send you the model to have a look at, perhaps you could provide me with an email address to send to?

Thanks again,
Sam

 

[IceBreakerSours]

If any of it is or has been for course-work, do NOT send it. Otherwise, send a compressed CAE here: orthofea!/!at!/!gmail!/!dot!/!com


Check the manuals.

You want to check ALLSD and ALLSE for Whole Model. ALLSD should be a fraction or less of ALLSE particularly near the sharp transition in the stress-strain curve (which, if I remember your model correctly, is near the end of simulation time in step 1). And finally, ALLSD should go back to zero or something very small. Otherwise, the results may be unreliable. Again, read the manuals for details.

FYI: Non-linearities can be a time bomb, as I like to put it, if one does not fully understand what one is dealing with. Further, just because your model converges does not mean it is correct. You have two non-linearities present in the model: Material non-linearity and boundary non-linearity. And if there is large deformation/rotation, then geometric non-linearity is also present in the model. By the way, if there is large deformation/rotation, then you must turn on the NLGEOM parameter, which is an option present in the STEP definition.

http://www.eng-tips.com/faqs.cfm?fid=376