View Full Version : Analytical Rigid Part
I'm kinda new to Abaqus and have just started using it a few days ago.
This is a brief description of my simulation.
I'm trying to compress a deformable sphere which is placed between 2 Analytical Rigid bodies. The flat rigid body at the bottom is fixed (ie. ground) and the one at the top will be compressing onto the sphere in a downward motion.
I tried to apply pressure on the Rigid body (to compress the sphere) at the top by selecting it in the viewport. However, I was told that it's not possible. Is this true?
Are there any other ways to go around this problem if it's true?
Thank you so much!
Yes, I believe it when you say that you cannot apply a pressure on a rigid body. Rigid bodies in ABAQUS only have 6 degrees of freedom (3 displacements and 3 rotation angles). The degrees of freedom of a rigid body are assigned to a reference node. As you know, a node also has exactly 6 DOF. The complete motion of the rigid body is controlled by the movement and rotation of its reference node.
The work around in your case is to apply a concentrated force on the reference node of the rigid body.
Best of luck,
Thank you so much for your reply!
I have another problem at hand.
I'm trying to simulate the aspiration (sucking) of a deformable sphere into a pipette (cylindrical tube, analytical rigid).
I'm comparing Hyperelastic Neo-Hookean model with Elastic Linear model. If the units that I used in creating the parts is in microns, do I need to adjust the Young's Modulus too? (For eg. if Young's modulus for the sphere is 500 Pa, do I enter the value as 500 or 500e-12?)
For assembly, I merely translated the sphere such that it 'sits' right on the top opening of the pipette, with the underside of the sphere exposed to the pressure that I will apply later.
For interaction, I made the inner surface of the pipette as the master, and the outer surface of the sphere as slave. The property is Frictionless.
For boundary conditions, I fixed the pipette in all DOFs, and the top half of the sphere in YASYMM (Y-antisymmetry) to prevent the sphere from 'rolling' around. I am not sure if this is the right way.
For loading, I would like to apply pressure (do I have to adjust the units here like the Young's Modulus?), on the surface of the sphere that can be seen from inside the pipette. To do this, I had to partition the sphere so that I can select separate surfaces rather than the entire sphere surface. Again, I'm not sure if this is ok. Is there any other way to apply pressure in the pipette? Because as the sphere is being sucked into the pipette, the surface area might be changing.
For meshing, the element shape was tetrahedra. The element type was C3D4H (Standard, 3D Stress, Linear, Tetrahedra, Hybrid formulated, No distortion control). Can it be improved to suit a sphere?
After analysis, I noticed that the nodes at 0, 90, 180, 270 degess (when looking from the bottom) were not able to 'flow' inside the pipette, thus causing high distortion to the surrounding elements. Some of the elements also managed to 'cut' into the pipette.
I am not sure if this is due to partitioning I created when selecting the surface for applying pressure, the meshing, the material property and loading units, the Step, or the type of part (solid,shell,etc)?
Ideally, I would like the entire sphere to 'flow' into the pipette.
I am sorry if I did not provide enough information as this is still my first couple of days of using Abaqus! Here are some of the images.
Most of your modeling efforts sound right. Here are a few comments:
:arrow: You need to be very careful when chosing units. I wrote a document summarizing a few different sets of consistent units that is available on the downloads page. If you use micron as a length dimension, then you will need to use consistent pressure and modulus values. This is very important.
:arrow: I would not model the whole geometry like you did. Due to the quarter-symmetry it is sufficient to simulate a 1/4 of the model. If you look down the pipette from the end then each of the four quadrants (0, 90, 180, 270) are symmetricial and it is sufficient to model one of these. Using symmetry in this case will make your simulation run 4 times faster while at the same time give exactly the same results. Using the quarter-symmetry will also make it easier to apply the boundary conditions correctly.
:arrow: The one thing about your problem that is difficult to simulate is the applied pressure loading conditions. Right now I cannot think of a good way to apply the pressure on the interior sides of the sphere, as you said, the interior region will change with time. I suspect, however, that the error introduced from simply applying pressure on the initial region that is inside the pipette might not be too large.
Thanks Jorgen for your advice! I have read your document regarding the units and it was very helpful.
I have reduced it to a 2D planar model. And this is the result that was achieved.
The strange thing is that I was still unable to suck the entire cell into the pipette. I have tried applying a larger pressure and widening the opening of the pipette but none of them worked.
I have another question to ask. I would like to connect one instance of a part to multiple instances of the same part, such that they will 'stick' to each other and not break away, like in this case :
I tried to apply Join in the Interaction module, but was not able to select more than 2 points on 1 instance (Ref point and vertice).
Also, how do I choose the master and slave surfaces if they are all of the same material?
Thanks for taking the time to read! And sorry for the novice questions!
I like your images: interesting simulations.
Here are answers to your questions.
(1) In order to enable the cell to get sucked you need to run the simulation using an explicit FE code, such as ABAQUS/Explicit. An implicit simulation will not be able to "go past" the instability/onset of "suck-in".
(2) To make different parts "stick", I recommend that you use contact with the "tied" option. You will need to specify all individual contacts.
(3) Finally, you can select the master and slave surfaces from the same part with the same material. All you have to do is to partition the part into the desired regions.
I have a question about symmetry after reading this. I am using Abaqus to model a diamond tipped indenter scratching the surface of polymer composite. The polymer is basically a 3D deformable plate, but I am trying to declare the indenter (consisting of a cylinder with a conical tip) as a analytical rigid body, but cannot revolve it around the center line since abaqus gives me the warning (object cannot have side on center line). Do you think it would be plausible to break this model into half (basically looking at a cross section), considering that my plate and indenter are symmetrical?
Yes, it sounds like you can use symetry!
Powered by vBulletin® Version 4.2.0 Copyright © 2013 vBulletin Solutions, Inc. All rights reserved.