Breast simulation: Deformation Map 1

[pjuneja]

Hi,

I want to simulate the deformation of breast under gravity. I initially have patient's breast images in one position (supine, with breast falling on the chest). I want to apply gravity loading and simulate breast image in another position (prone, with breast falling away from the chest).

I follow the standard path i.e. segment images (supine data), generate mesh, import the mesh into ABAQUS, apply material properties, BCs and loads and run the simulation and I get deformed breast mesh (simulated prone).

My query is once I have done deformation simulation how do I extract imaging data from the simulation result (deformed Mesh)? I hope the question make sense. This would be needed for number purposes including generating the deformed image data set.

Is it possible to export/obtain deformation map in ABAQUS?



Thanks

Prab

 

[IceBreakerSours]

In order to model prone position I would expect either a boundary condition (or an interaction) to be applied to the breasts to model contact with table unless there is a space in the table which allow the breasts to hang under gravity loading.

Anyway, I guess you mean to ask how to extract the deformed mesh. I think Dave's suggestion in the Yahoo! group is spot on. You may export the ODB into one of the formats that your program likes (VRML, OBJ, STL..) or you may write a Python script that extracts the nodal coordinates out of the ODB.

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

 

[rstupplebeen]

Reverse engineering from one position to another will be difficult since the initial position is not a stress free state. A while back I helped someone try to create the undeformed geometry which would then be loaded. Please check out that thread here which was cryptically named.

http://www.eng-tips.com/viewthread.cfm?qid=306126.

I hope this helps.

Rob Stupplebeen

https://sites.google.com/site/robertkstupplebeen/

 

[pjuneja]

Thanks for the responses I thought I had replied here ealier but not.

My doubt here is not about model as am currently using model from literature and set-up system that we can use to do breast deformation simulations. What I want is to be able to map material points from the deformed mesh to orignal image-set (3D matrix with each voxel value represting image intensity at that point), so that the deformed image-set can be generated and used.

Someone suggested extracting a list of nodal coordinates in the deformed and
undeformed configurations night help me to export something like deformation map. This deformation map might help to generate deformed image-set (simulated images) from the undeformed image.

I am not entierely sure how would I do it, but will give it a try.

thanks
Prab

 

[IceBreakerSours]

I see just one warning (c3d4h and c3d10i .. ) and I don't see any cause for concern. However, I have some general comments about the model:

1. To my eyes, the mesh does not make it look like a breast at all because of non-smooth outer geometry. Its just my opinion; it may be okay for the application.

2. Are you consistent in your units? The density is 1e-09, gravity is 9800, and C10 is 0.0001625.

3. As Dave suggested, I would've gone with C3D10H elements instead of C3D4H. C3D4 does not have sufficient degrees of freedom.

4. The model seems to run just fine. What is tricky is to verify AND validate the model. As someone put it, verification means "Is the sum right?" and validation means "Am I doing the right sum?"?

5. What area of the breast tissue and what field variable (stress, strain, displacement, pressure, etc.) is of interest to you? Since the geometry is quite simple, don't forget to do a mesh convergence study for the variable at the location of interest (after having verified the model) and then validate it against imaging data. For example, max. displacement is ~ 15 units. Is that a sane number? Can you give some images a quick cursory look and see if that number falls in the ballpark? Once these numbers make sense, you can move on to validation of the field variable.

6. A few elements at the top are getting heavily distorted. If that region is critical, ensure appropriate aspect ratio for those elements.

7. Also, I'd definitely double-check the following:

a) Material parameters (Are the units consistent?).
b) Boundary condition (By the way, there's no need for ENCASTRE; PINNED is sufficient for continuum elements).
c) Loading condition (Are the gravity vectors pointing in the correct directions?).

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

 

[pjuneja]

Thank you for very helpful and comprehensive comments.

1. Mesh geometry is derived from the imaging data and based on clinician outlining of breast, I agree with its not quite smooth. I struggled a bit to generate mesh from the 3D imaging data and in the end used iso2voxel, tetrahedral mesh generator, tool available free online. Though initially I wanted to use voxel based meshing (hexahedral elements) but didn't find a suitable generator.

2. Just double checked units, its fine, am using SI (mm) as my mesh units are in mm.

3. I have started to use C3D10 elements after Dave's suggestion.

4. I agree with you and that's the goal point of my current work i.e. to validate breast deformation model, and then use it for application deformable registeration. I will validate using prone-supine data. For validation I asked the question at start of this thread (deformation map).

5. I am interested in displacement of breast tissues. As I run these simulation am keeping an eye on displacement and am making sure the breast length is as expected and also looking out for abnormal tissue displacement. After this I will validate the model, by simulating prone images. Mesh convergence study would be important too, though earlier I didnt know this is what it was called !.

6. That's one difficulty am facing, as to how to do adaptive meshing? Because in some case the results don't converge because of excessive distortion in some elements.

7. I double-checked these.

Thanks
Prab

 

[IceBreakerSours]

1. What did you use to create the 3D geometry? MIMICS/Simpleware/3D-Doctor/Slicer 3D/..? I bet there must be some option to smoothen the geometry; you should try that.

If you can't make it, the best way is to make the geometry using SolidWorks-like programs. Import a few images at appropriate distances, carve out splines along the regions of interest and create a boundary or a loft feature! This way you get very nice and smooth geometries.

Also, why don't you import the geometry in to CAE and mesh it using ABAQUS? ABAQUS can do a good job at generating tet mesh. Heck, if you relax some geometric constraints, it may even generate a hex mesh (C3D20H) for you. IA-FeMesh can also do this job quite well since the geometry is very easy to mesh.

3. Try refining the mesh.

4. Correct me if I am wrong. I guess what you want is to be able to export the deformed geometry from the ODB, correct? If so, you have a few options:

a) Upgrade to ABAQUS v6.12.
b) As Dave suggested in the ABAQUS Yahoo! Group, extract nodal coordinates using a Python script. Use this nodal coordinates (point cloud) to make the deformed geometry in some software like AutoCAD, SolidWorks, etc.

6. If the distorted elements are away from the region of interest, there is no need to for adaptive meshing. If you really need it, check the examples in the documentation; its quite straightforward.

7. I think too many nodes are fixed (using ENCASTRE). But then, I don't know the problem very well so you may have it right.

By the way, continuum elements have no rotational degrees of freedom. So, fixing rotational degrees of freedom is irrelevant/redundant. PINNED is just fine for the job.

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

 

[pjuneja]

1. I used iso2mesh (

http://iso2mesh.sourceforge.net/cgi-bin/index.cgi)

to generate mesh from imaging data. After importing this mesh into ABAQUS I used a plugin to extract geometry and I re meshed this geometry. Currently, I find this one limiting me to do homogeneous breast model only (not heterogeneous: fat and fibroglandular tissue). Even then I am doing this because of the difficult in getting geometry from medical images in ABAQUS. I looked into various things to get my geometry/mesh but in the end iso2mesh seemed good way as its automatic and it does create multi-domain meshes (heterogenous breast), though currently am not able to use them.

I have tried 3D-doctor, the files (tried both IGS and STL) it wrote didnt open in ABAQUS. When I tried Slicer 3D with IA-Mesh functionality to mesh the breast, I think I encountered some limitation on number of elements. MIMICS/SIMPLEWARE are just too expensive for my grant. I will try to smooth my surfaces.

4. It might be odb or deformation at nodes, am not sure about this, I will try it and see.

 

[IceBreakerSours]

1. As I mentioned in my previous response, the simplest way is to make the geometry (using loft or boundary feature) in SolidWorks. All you need to do is to:

a. Create a few planes with a known distance from each another
b. Go to Sketch
c. Import the MR images (Tools->Sketch Tools->Sketch Picture) in to each plane.
d. Resize the images to a known distance (i.e., calibrate) between two points.
e. Use spline feature to create a smooth outline of the breast tissue.
f. Use boundary feature (or loft) to create the 3D geometry.
g. Save it as a .sat or .step file.
h. Import the saved file as a Part in to ABAQUS/CAE.

This will save you a LOT of headaches down the road. You can make quick changes to the geometry if the need arises, you can refine the mesh for a mesh convergence study with a short turnaround, and the quality of the hex mesh will be excellent.

4. Besides all the options suggested to you so far, you can repeat the process in #1 above to get the deformed geometry. The only difference is that this time around you'll be using screenshots of model section cuts as images.

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

 

[pjuneja]

Thanks, it sounds like very good solution, I will try it soon.
Prab