Eng-Tips is the largest engineering community on the Internet

Intelligent Work Forums for Engineering Professionals

Register Log in
  • Congratulations waross on being selected by the Tek-Tips community for having the most helpful posts in the forums last week. Way to Go!

too many increments, warped and distorted elements 1

Status
Not open for further replies.
MrSamuel

MrSamuel

Bioengineer
Oct 13, 2011
45
0
0
CA
I have a model of a human foot that consists of rigid bones kinematicaly connected and enveloped in linearly elastic soft tissue. Ligaments are approximated as tension only trusses.

The model is finicky, slight changes can prevent the model from solving. I get the error "too many increments" and get the "distorted" and "warped" warnings. But I get those warnings when it solves too. Really, the warnings are the exact same whether or not it solves. So how am I to know what is going wrong? Any recommended trouble shooting steps?
 
Replies continue below

Recommended for you

Sort by date Sort by votes
If those elements are "away" from your region of interest, then you need not bother too much. If the model is finicky, double-check the boundary/loading conditions, units, material assignment, contact, etc. Look at the warnings in the files and in Job Diagnostics for clues. If everything else checks out fine, then you could edit some of the nodal coordinates of problematic elements in such a way that the deformed elements end up looking like cubes.

If there are any subroutines, test the code outside of ABAQUS, then in ABAQUS on a unit cube and then on a larger-sized cube before running it with your model.

 
Upvote 0 Downvote
The soft tissue is connected to the bones with tie constraints. I'm having better luck getting it to solve when I turn off "adjust slave surface initial position". This to me suggests that the fragility of the model is in fact due to the warped elements. I will continue to improve the mesh structure. Abaqus is frustrating in that two versions of a model can run with the exact same warnings, but one converges while the other does not...

I seem to be on the right track for now, thanks for your help, once again!

Sam
 
Upvote 0 Downvote
The soft tissue was created by a boolean difference operation between the skin geometry and the bone geometry (boolean was done in Rhino3d). Thus the tied surfaces should be very close. But I don't think the nodes coincide. Merging would do this? How could I merge them?

Turning off "adjust slave surface initial position" allows it to solve, though a lot slower for some reason.

Sam
 
Upvote 0 Downvote
The bones are shells with rigid body constraints. I use the rigid body constraints to also pin the ligaments and fascia to the bones. If I merge the bones and soft tissue into one part, then I don't think I can apply rigid body constraints to the individual bones and then attach ligaments and fascia. Right?
 
Upvote 0 Downvote
I don't see that there is a way to use rigid body constraints only part of a merged part, so don't think that's an option for me.

Turning off "adjust slave surface initial position" quadruples solution time, give or take an uple. As I understand, the function adjusts nodes that are tied by moving the slave nodes to the master, thereby altering the mesh. I think I run in to problems because my mesh gets distorted when this happens. I get that. But I don't understand why turning the function off would result in so much longer solution times. Any explanation?

Thanks,
Sam
 
Upvote 0 Downvote
You can assign a rigid body constraint to a section of a part.

IF you are following the guidelines provided by ABAQUS (Analysis Manual) in defining the tie constraint, then I do not know the answer to your question without looking at the model. Multiple nonlinearities can drive the default solver nuts.

a) Try the unsymmetric solver (helpful in contact related convergence issues).
b) If this isn't the case already, see if assigning linear elastic materials to all tissues.

 
Upvote 0 Downvote
"You can assign a rigid body constraint to a section of a part."
I've used the tie option in the rigid body constraint on each bone surface rather than selecting the entire bone body with the body option. I think this is what you meant.

I merge the soft tissue with a bone and then mesh the merged part with the bone as quad shell and the soft tissue as tetrahedral. When I run it, I get the error:
THE FACE SHOULD BE ONE OF THE FOLLOWING: S1, S2, S3, S4, S5, S6, SPOS, SNEG, END1, END2, E1, E2, E3, E4 OR EDGE
What does this mean and how can I get rid of the error?

I will try unsymmetric solving.

Thanks,
Sam
 
Upvote 0 Downvote
I was able to use the body elements region type after I turned on "retain intersecting boundaries" when I merged the soft tissue and bone.

I see MPCs for beams, ties, links and a few others, but nothing to do with transition zones. I do see a constraint for shell to solid, is that what you mean?

I'm thinking it might be easier to just model the bones as rigid solids. I tried it for one of the bones and it appears to work. I was only modeling with rigid shells to reduce the total number of elements.

Thanks,
Sam
 
Upvote 0 Downvote
I have been modeling the bones as solid as you suggested. I was using rigid body constraints on the bones as I don't need to see stress and deformation of the bones is negligible. However, I'm noticing the model is more efficient if I just leave the bones as deformable solids. Is this again because nonlinearties or discontinuities occur at the border between the elastic soft tissue and rigid bone? Perhaps I should just mimic rigid by applying a high youngs moduls to the bone?

I was using the rigid body constraint for other purposes too:
-to pin the ends of the ligaments and fascia (tension only trusses) to the bone
-to tie reference points for connecting the bones via pin joints and hinge joints
-to tie reference points for applying boundary conditions (at the ankle) and forces (on the calcaneus to simulate achilles tendon force)

If I'm not going to use rigid body constraints for these, what is the next best option, couple or tie, or something else? What do you think is the best technique for pinning or tieing a point to a solid?

Your help is very much appreciated!
Sam
 
Upvote 0 Downvote
MrSamuel said:
Is this again because nonlinearties or discontinuities occur at the border between the elastic soft tissue and rigid bone?
Click to expand...

Displacement discontinuity or constraints can, in some situations, result in ill-conditioning of matrices and poor convergence rates.

Young's Modulus of 16 GPa for cortical and 400 MPa for cancellous bone are typically used in continuum models.

MrSamuel said:
What do you think is the best technique for pinning or tieing a point to a solid?
Click to expand...

Unless you must allow the ligament to rotate (which, to me, makes no clinical sense), merge the ligament node to the nearest node on a bone. Saves you from messing with constraints.

Other options are MPC Tie and Kinematic/Distributing Coupling constraints.

 
Upvote 0 Downvote
IceBreakerSours said:
merge the ligament node to the nearest node on a bone
Click to expand...
How do I do this? In the assembly module using instance/merge? But then I cannot see the nodes because I'm not in the mesh module. Also, I've merged the bones with the soft tissue, so I can no longer distinguish between the bone mesh and the soft tissue mesh.

If I decide to go the MPC tie constraint route, I am first asked to select the MPC control point and then the slave node region. In this case I would think my bone should be the control and the ligament end nodes should be the slave region. But the bone is a part, not a control point. How should I set this up?

Thanks,
Sam
 
Upvote 0 Downvote
I am not entirely sure if this will work but try the following in your INP:

Code: 
*MPC
TIE, instanceName.Node#, instanceName.Node#

The "dot" in instanceName.Node# necessary. If this does not work, then the nodes must be merged.

Perhaps I am missing something but why do you need to see the nodes once the nodes are merged? All you need to do is ensure property material property is assigned to the ligament and the bone.

This whole process of merging instances may mean more work for you now but it saves you a lot of headaches down the road.

 
Upvote 0 Downvote
I'm having some luck merging the instances.
A problem I am having is that I cannot see the bones in the visualization module (results) as they are a single part merged with the soft tissue. I need to be able to see the bones to inspect their relative movement.
I've tried to use transparency, but you can only see elements on the outside surface of a part.
I can look at a cross section and view by materials or sections and thereby distinguish the bone, however a single cross section isn't enough, I need the full 3D view of the bones.
Any suggestions on how to view the bones?

Thanks,
Sam
 
Upvote 0 Downvote
If the bone and ligament are one part, you should be able to see the whole part, shouldn't you? Unless I am missing something, merging has nothing to do with appearance of regions in the Visualization module. Perhaps you need to change some options in the Visualization module. I would try running the model or opening the ODB on another machine or version of ABAQUS.

 
Upvote 0 Downvote
Status
Not open for further replies.

Similar threads

hussain98
  • Locked
  • Question
Too many attempts made for this increment
Replies
1
Views
14
FEA way
FEA way
MF Afif
  • Locked
  • Question
Abaqus Machining Simulation: Highly distorted element on breaking chips
Replies
3
Views
13
FEA way
FEA way
Smadar11
  • Locked
  • Question
ABAQUS- stractural model- fine elements in crack area
Replies
3
Views
26
FEA way
FEA way
SinaPeugeot
  • Locked
  • Question
Bending-Only Shell Elements in Abaqus/Explicit
Replies
3
Views
22
SinaPeugeot
SinaPeugeot
Fblthp
  • Locked
  • Question
Abaqus How to show the coordinate system of beam elements in visualization window?
Replies
3
Views
42
FEA way
FEA way
Back
Top