too many increments, warped and distorted elements
too many increments, warped and distorted elements
(OP)
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?
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?





RE: too many increments, warped and distorted elements
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.
http://www.eng-tips.com/faqs.cfm?fid=376
http://www.eng-tips.com/faqs.cfm?fid=1083
RE: too many increments, warped and distorted elements
I seem to be on the right track for now, thanks for your help, once again!
Sam
RE: too many increments, warped and distorted elements
http://www.eng-tips.com/faqs.cfm?fid=376
http://www.eng-tips.com/faqs.cfm?fid=1083
RE: too many increments, warped and distorted elements
Turning off "adjust slave surface initial position" allows it to solve, though a lot slower for some reason.
Sam
RE: too many increments, warped and distorted elements
I can't say for sure but as long as the results make sense and the tie constraint is away from the region of interest, "a lot slower" may very well be alright unless you are talking about going from minutes to days.
http://www.eng-tips.com/faqs.cfm?fid=376
http://www.eng-tips.com/faqs.cfm?fid=1083
RE: too many increments, warped and distorted elements
RE: too many increments, warped and distorted elements
http://www.eng-tips.com/faqs.cfm?fid=376
http://www.eng-tips.com/faqs.cfm?fid=1083
RE: too many increments, warped and distorted elements
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
RE: too many increments, warped and distorted elements
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.
http://www.eng-tips.com/faqs.cfm?fid=376
http://www.eng-tips.com/faqs.cfm?fid=1083
RE: too many increments, warped and distorted elements
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
RE: too many increments, warped and distorted elements
The error is because of the shell to continuum element transition. Search for MPCs for transition in the Analysis User's Manual.
http://www.eng-tips.com/faqs.cfm?fid=376
http://www.eng-tips.com/faqs.cfm?fid=1083
RE: too many increments, warped and distorted elements
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
RE: too many increments, warped and distorted elements
Shell-to-solid coupling
Search these terms ^.
It would be convenient to model bones as solids because merging (while retaining boundaries, which I forgot to tell you about) will allow continuity in the solution (i.e., displacement).
http://www.eng-tips.com/faqs.cfm?fid=376
http://www.eng-tips.com/faqs.cfm?fid=1083
RE: too many increments, warped and distorted elements
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
RE: too many increments, warped and distorted elements
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.
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.
http://www.eng-tips.com/faqs.cfm?fid=376
http://www.eng-tips.com/faqs.cfm?fid=1083
RE: too many increments, warped and distorted elements
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
RE: too many increments, warped and distorted elements
CODE --> ABAQUS_INPUT_FILE
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.
http://www.eng-tips.com/faqs.cfm?fid=376
http://www.eng-tips.com/faqs.cfm?fid=1083
RE: too many increments, warped and distorted elements
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
RE: too many increments, warped and distorted elements
http://www.eng-tips.com/faqs.cfm?fid=376
http://www.eng-tips.com/faqs.cfm?fid=1083
RE: too many increments, warped and distorted elements
Any thoughts?
RE: too many increments, warped and distorted elements
You must have defined element sets assigning appropriate material properties. Go to Create Display Group and isolate those element sets for visualization.
http://www.eng-tips.com/faqs.cfm?fid=376
http://www.eng-tips.com/faqs.cfm?fid=1083
RE: too many increments, warped and distorted elements
I'm just about there. I just need to connect the bones. I'm doing it kinematically with pins and hinges rather than contact modeling (trying to make this thing fast).
In the example of a hinge joint, I create two reference points. The first point lies somewhere on the hinge axis. I create a coordinate system at this first point with the X-axis pointing along the hinge axis. A wire connects the two reference points, and I assign a hinge connector to this wire. Finally, I connect one reference point to one bone, and the other reference point to the other bone. I was doing this connection within the rigid body constraint, but now that I'm not using rigid body constraints, what is the best tool? Couple, tie, MPC tie or pin? I tried tieing the reference point (master) to a single bone surface, but this didn't constrain relative bone motion to the hinge axis. How could I do this? Is there a totally different and better approach I should try?
What confuses me is that I am trying to constrain a reference point to a deformable solid. Perhaps I should be trying to constrain it to a single node. I'm not sure how this is done and even if I achieve it, its not a very robust solution because I have to redo the connection every time I rebuild the mesh during convergence testing...
Thanks!
Sam
RE: too many increments, warped and distorted elements
Use this scheme: Bone-"MPC Pin"-Bone
Pick one node (appropriately located) on each bone and assign MPC Pin between those two nodes.
http://www.eng-tips.com/faqs.cfm?fid=376
http://www.eng-tips.com/faqs.cfm?fid=1083
RE: too many increments, warped and distorted elements
-When creating a node set in the mesh module, I can only see external nodes, not the interior ones (kind of like the problem I was having with the visualization module). How can I select an interior node? How can I select the node nearest a 3D coordinate I specify (I know before hand the center of rotation)?
-If I remesh the part for convergence testing, won't I loose the sets and have to re enter them all?
-While I was testing working with nodes, I created an encastre boundary condition on a node set, yet the node still moved, any guess why it wouldnt hold still?
-In regards to MPC pin constraints, when I have two bones A and B with respective internal nodes A and B, I create a MPC pin constraint with node A as the control and node B as the slave. Rotations occur about both node A and node B (oddly, this is the case for MPC tie constraint too, I don't see the difference between tie and pin). What I really want is for both bones to rotate only about node A. How can I do this? Perhaps I need the slave node set to contain three nodes in bone B? Or is there an easier way?
Hope this is clear enough,
Thanks,
Sam
RE: too many increments, warped and distorted elements
CODE --> ABAQUS_INPUT_FILE
So, all you need to do is ensure you know the node numbers. And even when you are trying to carry out convergence testing, the same procedure applies.
If I remember correctly, ABAQUS has a plug-in which lets you detect a node closest a set of coordinates. If its not installed, you may find it on the SIMULIA custhelp website.
A fixed node can not move. Double-check your model.
Can't you simply fix rotational DOFs of node B? For example, the following fixes 5 and 6 rotational DOFs:
CODE --> ABAQUS_INPUT_FILE
http://www.eng-tips.com/faqs.cfm?fid=376
http://www.eng-tips.com/faqs.cfm?fid=1083
RE: too many increments, warped and distorted elements
http://www.eng-tips.com/faqs.cfm?fid=376
http://www.eng-tips.com/faqs.cfm?fid=1083
RE: too many increments, warped and distorted elements
I'm thinking I should try the connectors again. They worked find for me previously when I could add the reference points to rigid body constraints. But now that I'm not using rigid body constraints, I'm not sure how to tie the reference points to the bones (I haven't had much luck with couple and tie constraints) ... Have you used connectors like this before, how would you set up a hinge connection between two deformable bodies?
Thanks for all your time on this, a lot of questions I've had... I hope others will happen across this thread as you've provided some excellent advice.
Sam
RE: too many increments, warped and distorted elements
You make all sorts of changes you want in the CAE, create an INP and then edit the generated INP only where changes are needed. You don't have to repeat anything (although there are exceptions).
I'd kinematically couple (while fixing DOFs I want fixed) all nodes (except the ones that are assigned to some other constraint) of each bone to a reference node. Then, I'd use MPC Pin type constraint between the two reference nodes.
I've used connectors mostly, if not always, for actuation (e.g. in modeling the effect of muscles.)
http://www.eng-tips.com/faqs.cfm?fid=376
http://www.eng-tips.com/faqs.cfm?fid=1083
RE: too many increments, warped and distorted elements
Heres a question in a slightly different direction. Please let me know if I should create a new thread for it, though the answer may be very short.
I push a flat hexahedral meshed solid into the foot to simulate loading on flat ground. Pressure is what I am interested in, so I look at CPress on the ground model. I thought the results looked high, so I multiplied the pressure at each node by the element area to calculate force. Sure enough, I got a force higher (it varies depending on mesh density, but maybe around 20%) than what was applied during loading.
Any idea why it is off? Do you know, or know of a reference that explains how CPress is calculated?
Thanks,
Sam
RE: too many increments, warped and distorted elements
a) If the ground is supposed to be far more stiff relative to the bone, then why not simply create an analytical rigid surface for the ground?
b) You are not taking in to account the shear stress, are you?
I am not sure if this is possible but check what RF (at the ground nodes that are in contact with the foot or the other way around) gives you.
I don't remember off the top of my head how CPRESS or CSTRESS are computed by ABAQUS but I am sure the Analysis User's Manual must have sufficient content related to this. Also, you might want to watch the CPRESS error indicator (CPRESSERI; CSTRESSERI). The error value should be a fraction of the contact pressure in the region of interest.
How did you compute element area? Note that ABAQUS must use some sort of threshold to define when a surface comes in to contact with another surface. Based on that distance, it will decide how much "area" is in contact. There is an output variable for contact area and I guess its CAREA; check the manual. Then, after computing the solution, it must compute a vectorial resultant force on the area. Finally, there is nodal averaging (in the Visualization module) to be kept in mind as well.
http://www.eng-tips.com/faqs.cfm?fid=376
http://www.eng-tips.com/faqs.cfm?fid=1083
RE: too many increments, warped and distorted elements
Thanks for getting me on the right track, again!
That's all for now.
Sam