×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

too many increments, warped and distorted elements

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?

RE: too many increments, warped and distorted elements

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.

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

(OP)
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

RE: too many increments, warped and distorted elements

(OP)
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

RE: too many increments, warped and distorted elements

(OP)
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?

RE: too many increments, warped and distorted elements

(OP)
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

RE: too many increments, warped and distorted elements

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.

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

(OP)
"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

RE: too many increments, warped and distorted elements

(OP)
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

RE: too many increments, warped and distorted elements

(OP)
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

RE: too many increments, warped and distorted elements

Quote (MrSamuel)

Is this again because nonlinearties or discontinuities occur at the border between the elastic soft tissue and rigid bone?

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.

Quote (MrSamuel)

What do you think is the best technique for pinning or tieing a point to a solid?

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

(OP)

Quote (IceBreakerSours)

merge the ligament node to the nearest node on a bone
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

RE: too many increments, warped and distorted elements

I am not entirely sure if this will work but try the following in your INP:

CODE --> ABAQUS_INPUT_FILE

*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.

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

(OP)
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

RE: too many increments, warped and distorted elements

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.

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

(OP)
The bone, soft tissue, and ligaments are one part. Its the bone and soft tissue being merged that is the problem. Once they are one part, I cannot isoloate the bone componement for visualization. And the surfaces of the bone don't exist anymore, only the surface of the soft tissue as the bones are inside the soft tissue. See in the attached pic how you can see the tibia and fibula bone where they are outside the soft tissue, but where they are inside they are no longer visible.
Any thoughts?

RE: too many increments, warped and distorted elements

(OP)
Brilliant, I can see the bones now!

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

(OP)
To pick a node, I go to the mesh module, select the main part (merged ligaments, bone, and soft tissue), and create a set. I do this for two bones (I'm just making one pin connection for now). I then go to the interaction module and create an MPC constraint, select the first set (control node), then the second set (slave node), I then specify the MPC type to be pin. Is this the correct procedure? Assuming it is, here is where I have trouble:

-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

Sometimes it is easier to work with INPs directly. I'd simply put the following lines in the INP where you have your other constraints defined (assuming the nodes belong to the same part):

CODE --> ABAQUS_INPUT_FILE

*MPC
PIN, Node a, Node b 

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

*Boundary
node B, 5, 5
node B, 6, 6 

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

(OP)
Everything is great except for creating the bone to bone hinge and pin joints. I would really prefer not to work with the inp file as any changes to the cae file I make means I have to make changes to the inp file again. Just doesnt seem robust to me. And I'm having trouble tieing rotational degrees of freedom about a node with MPC tie constraint, it seems to work the same as MPC pin.

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

Quote (MrSamuel)

as any changes to the cae file I make means I have to make changes to the inp file again

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

(OP)
OK, I think I've got all the techniques you've helped me with working individually, now I just need to put it together in one moodel. Already I can tell it will be a fast and robust model.

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

Glad to hear that.

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

(OP)
With your help I think I figured it out: pressure listed at a node is not necessarily acting on an area the size of the element; at the edges of the contact areas, it will inevitably be less. Thus I cannot simply multiply each pressure by the element area and sum them to get total force. Though by reducing the ground mesh, this method approaches the actual force. This isn't the case for reaction force where summing the values at the nodes accurately results in total load regardless of mesh size.

Thanks for getting me on the right track, again!
That's all for now.
Sam

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources