Problem with Simulation of MIcropipette aspiration in Abaqus

[Amir]

Hi


I want to simulate the suction of a cell into a pipette, I saw a fellow called Sarius had the same problem here in 2005 but there was no clear solution to his problem that could help me either and neither I could find his/her contact to ask for help. :(

My model consists of a analytical rigid pipette and a spherical cell modeled axisymmetrically :
Properties : Viscoelastic (SLS)
Interaction :
frictionless
Hard contact

1- If I want to exert the instantaneous pressure I will face sever element distortion that even ALE adaptive meshing hardly can take care of it and also cell penetrates the pipette(although mesh is very fine in its neighborhood and hard contact is chosen) and if I don’t want to exert instantaneous pressure then I can’t see the elastic jump of the cell into pipette(which occurs upon instant suction pressure) and even in a non-instantaneous (ramp) pressure the cell still penetrates the master instance(pipette) which causes the process to fail.

In the case of sudden pressure or pressures with a sever ramp it seems that the cell is too soft for this magnitude of pressure because the deformation and length of cell penetrated in the pipette is far more than it should be and then after a while the job will be failed without success but I am sure that the constants are ok.

2-I have partitioned the cell edge in the opening of the pipette to exert pressure, and I know that the boundary of pressure is changed as the cell is sucked in. Is there any way to introduce the pressure not on the cell surface but in pipette? I mean so that we define a pressure be in the pipette and be exerted on whatever is located in it or near its opening like a sucking pipe?

3- I have read somewhere that there is a pdf provide by you to check unit transformations and scales in Abaqus in the download part but I couldn’t find it anywhere.

Links to photos that may help to have a schematic imagination of the model:
1- http://files.engineering.com/getfile.aspx?folder=b701fb87-7f6e-4d16-9700-63d1623e7cec&file=1.JPG

2- http://files.engineering.com/getfile.aspx?folder=55bd768e-91cc-40f4-9949-34b896f2b9c2&file=2.JPG



I would be more than very grateful for your help,
Yours Sincerely,
Amir

[Jorgen]

Interesting problem, and thanks for the images they were helpful :)

I would think that you start with the spherical cell in contact with the pipette and then apply a negative pressure on the surface of the sphere that is inside the pipette then you should be able to follow the displacement accurately. At this moment I cannot think of a clean way to introduce the pressure on the "surface of the pipette" as you mentioned.

The element distortion and contact problems that you mentioned should be possible to eliminate. Are you using Abaqus/Standard or Explicit? Are you using shell elements or solid elements for the spherical cell?

Here's a link to a document that discusses different sets of consistent units for FE analysis: FEM_Dimensions.pdf (http://polymerfem.com/polymer_files/FEM_Dimensions.pdf).

[biofriend]

HI

Thanks Jorgen,
I think that I am some steps closer to solve the problem.
What I need to learn now is mesh to mesh solution mapping which is not very clear in abaqus help for me.

[mukund]

hi amir,

have you found a solution to the problem of applying the suction in the micropipette rather than on the cell surface. would be very helpful if you could tell how you modeled this problem. I am new to abaqus.

thanking you,
mukund

[biofriend]

hi amir,

have you found a solution to the problem of applying the suction in the micropipette rather than on the cell surface. would be very helpful if you could tell how you modeled this problem. I am new to abaqus.

thanking you,
mukund


Hi

Unfortunately not. It seems that it is not possible with common modules and you might need to write a user script for pressure or something. At least I understood so after some trial and errors.
You may also be able to define the parts in eulerian form instead of lagrangian and mesh the internal space of the pipette, however this also seemed not to be that easy. In fact I just wanted to do this to see what happens, because even if you decide to put the pressure on the surface of the cell instead of defining it in the internal space of the pipette, the final difference in the displacement really seems to be negligible.
However if you are really eager to be ultra-precise, which in this type of problems is a little useless due to various sources of errors including experiments and FEM B.C's and etc. , you can try to update your pressure boundary condition after a couple of iterations manually under a mesh to mesh mapping algorithm. However I do not recommend this because It really is a waste of time and boring, except in special applications.



hi,

i came across your thread on simulation of micropipette aspiration on polymerfem.com. I am trying to model the same. the simulation stops within a fraction on the total step time because of excessive distortion of elements. i have applied non-instataneous (ramp) pressure. i would be grateful if you can help me out. i am new to abaqus.

-mukund

Do you use Explicit or Standard? I think MA is among the most cumbersome tests in cell mechanics literature to model. Try using standard instead of Explicit and try to get the meshes smaller near the fillet. Here are some general guidlines that may help you in your case, I would be happy to help further:

Take good care of contact regions, specially if you have a considerable tension concentration in these area, A finer mesh will be necessary to cover drastic changes in tension values.

Use 1st order elements instead of 2nd order if you know that a large deformation may occur. These are more persistent to distortion (and enhanced hour glass may be also a good choice). In /explicit ALE adaptive meshing may be a good help to avoid distortions.
I have seen that distortions may not only fail the analysis but even if the analysis in completed, the results might be reconsidered with caution.

if your solver is /explicit , a reasonable density value is critical. mass scaling should be always done with care. Flase parameters may lead to misleading results and most of the times, failure of the analysis. So check the units once again.

Cheers, Amir

[mukund]

hi,
i am using Standard. I followed the guidelines provided by you but am still getting the distortion error. would using ALE adaptive meshing in standard help?
i m using an elastic material.

thanks,
mukund

[biofriend]

hi,
i am using Standard. I followed the guidelines provided by you but am still getting the distortion error. would using ALE adaptive meshing in standard help?
i m using an elastic material.

thanks,
mukund


Hi
Sorry for the delay,

ALE is restricted to Explicit. The equivalent in standard is *Map solution, mesh to mesh solution mapping. I recommend avoid this as much as possible especially for large volumes of work. Only use it if you really have to. As far as I have experienced it, the most part of this procedure is manual and there is no guarantee that analysis will end successful, this means you may have to do it over and over again.

I have found out that in your case, the distortion, up to some degrees does not adversely affect the analysis and either the final disp. diagram but the tension is very sensitive to it.

use enhanced hour glass control for linear quad elements. These are more persistent to distortion.

make a partition on the right boundary of the cell(contact site) and increase the number of elements near the fillet and also places which will come into contact with fillet. The greater your suction pressure to E(pa) is, the more elements are needed at the contact sites with major bending and stretching for the solution to be able to converge.

I think, if you try to use hyperelastic Neo-hookean instead of elastic, your problem will possibly be solved.

Out of curiosity, what are you trying to do in your simulation? If its not accompanied with confidential matters.

Bests,
A

[mukund]

hi,
I have tried all your suggestions above. no matter what i change, the analysis is aborted when the cell reaches a particular deformation. I am planning to use mesh-to-mesh solution mapping. I was unable to find instructions for doing this in the abaqus manuals. can u direct me to an appropriate source.

my purpose for doing this simulation is mainly to learn abaqus.

thanks,
mukund

[mukund]

hi,
i am using mesh-to-mesh solution mapping. i have extracted the deformed shape and converted it into a part and meshed it. i have defined a new model and analysis job. for mapping the solution from the old mesh to the new one i have added *MAP SOLUTION to the .inp file of the new model. but how do i specify the mesh from which the variables are to be mapped? i could not find any arguments that could be specified with *MAP SOLUTION in the manuals. do i have to give some command or write a script after changing the .inp file?

thanks,
mukund

[biofriend]

.....
do i have to give some command or write a script after changing the .inp file?

thanks,
mukund


Hi mukund

What you've done so far is generally right, based on my experience. If I want to summarize the whole process, it can be so:

1- Run the job with request restart(you can find it under step and then in job modules)

2- When it fails then extract the deformed mesh and make a solid geometry and remesh it and make up the model again

3- Add map solution key word to the inp file : *MAP SOLUTION, STEP=step, INC=inc, UNBALANCED STRESS=STEP or Ramp

Step is the step from which you want to restart your job and the increment belongs to the the increment from which you have extracted your orphan mesh. i think its useful to note to extract your part from ODB in an increment before the critical and unshapely elements happens.
increments in ODB are called frame as far as I can remember.

4- Run it again from command window like this : abaqus job=newjobname Oldjob=oldjobname , You can set restart request in model attributes edit. You may need to do this over and over again, I mean each time you restart your analysis from a bit before the distortion becomes critical.



*** quadratic elements are better! Without them the process may fail! Due to element distortion and sever overclosure!

***Your elements in new model must be generally denser than your previous model for all the parameters to be mapped successfully or in some parts some of them may fail.

*** I think you might like to use preselected defaults in field and history outputs.

Finally, as before, I suggest you to leave mesh2mesh for your last option. Try to take care of your meshing and other parameters instead, unless you do it for learning purposes.

I hope you'll make it
Cheers,
A

[mukund]

thanks amir

the above was very useful.
just out of curiosity, can this process be automated by writing a script. if so, is the abaqus scripting manual sufficient for starters.

thanks,
mukund

[biofriend]

just out of curiosity, can this process be automated by writing a script. if so, is the abaqus scripting manual sufficient for starters.


You are welcome,

I personally have not tried that yet and I think that may be a bit challenging while the seeding and meshing the part should be done discreetly and in order to do it automatically you should find a robust rule of thumb for that, I mean where to place a partition on the boundary and number of seeds on each section and etc., but I don't think its impossible.

script manual of Abaqus seems fine of course I rather use MATLAB since I personally am more easy with that.

There also a lot of other resources on Python programming I'm sure.

Wish you luck,
A

[maria]

Hi Amir,

Thanks for the question. I have same problem here and thanks for explaining in details.

[bean0439]

Hi Amir,
I am very interesting about your works. I have the same problem as yours as I want to simulate the MA process for the chondrocyte. The material I used is just elastic because I am still studying about the viscoelastic properties for the chondrocyte and I want to make sure my model is working first but it is not. I used static, general step for my analysis, is that correct? Do I need to set up any other options for it? As you mentioned that you put the pressure on the partition of the cell. Could you tell me how to do it? How you make sure the pipette contact with the cell at the exact position in Assembly section and how you can partition the cell correctly? I am sorry if my questions are idiot because I am new to Abaqus as well as bioengineering.
Thank you in advance,

Steve