Assigning material properties to each element

[ardalansv]

Dear All,

I want to assign the material properties for each element using Abaqus. I am simulating bone and I want to assign the material properties of the bone to each voxel mesh using abaqus. The number of the elements I have is really high so I cannot manually select them. On the other hand, I need to use the UMAT subroutine to define the plasticity and damage criteria for my material. How can I assign to each element the material properties based on the bone fraction density or the hounsfield units (HU) that I am getting from the CT scans? I know there is a bonemat software which does that but my equations are different than theirs and I need to implement it probably using UMAT. Has anyone done this before. Please help me with this issue.

Regards,

Ardalan

 

[IceBreakerSours]

I am becoming more of a PowerPoint jockey than an Abaqus jockey lately so take these comments with a grain of salt:

*Distribution allows you to specify a spatially varying field. In your case, the field happens to be a material field. At the most, you may have to write a script to do some textual manipulation.

*********************************************************
Are you new to this forum? If so, please read these FAQs:

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

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[ardalansv]

Hello IceBreakerSours,
Thank you for your prompt reply. The *Distribution feature isn't for the 2D (shell) elements? I have hexahedral continuum elements.
Regards,
Ardalan

 

[adfergusson]

Its been quite a few years and I’m more of a powerpoint monkey these days too, but I’ve done something broadly similar with building models of composites from microscopy images (see photo). We have a program that would overlay a mesh on an image, identify the fibre orientation in each element of the mesh and then create a file that listed every node (plus it location) and the fibre orientation associated with each element. I wrote another program that would take this file and build an input deck for ABAQUS from it. To do this, my program would give every element its own node set, element set and material property card in the input deck. As every element has its own material property card, you can change the properties of each element. I did this so that I could have different fibre orientations and damage criteria for each element so this sort of approach should work for you too.

 

[adfergusson]

I’m guessing that you don’t have the ability to get fibre orientation data for the bone but I do have a cool idea (well, I think its cool) of how you could assign orientations/anisotropic properties to each element. Once you have your model built with every element having its own nset, elset, material, etc… you could then apply a ‘real world’ like load. You could then find the direction of the max principle stress for each element and then use this to assign an orientation and/or anisotropic properties to each element; virtual Wolff net bone remodelling!

 

[IceBreakerSours]

It works for solid bricks just fine. Please check the documentation.

*Distribution is the most efficient way of specifying spatially varying fields; other options, while aren't any more or less accurate, are less efficient.

*********************************************************
Are you new to this forum? If so, please read these FAQs:

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

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[ardalansv]

Hello IceBreakerSours,
I have read about distribution and discrete fields and how to make it in documentation but I don't know how to use it in material section. for example if I want to use various linear elastic material properties for let say a part made of 8 elements. How can I assign element number 1 modulus of 10 and Poisson's ratio of 0.3 and element 2 modulus of 100 and Poisson's ratio of 0.3 and so on?

Please help me on this since I am really confused!

 

[ardalansv]

Hello adfergusson,

This is exactly what I looking into applying in my model. Could you please guide me that how you did this?!
Thank you.

 

[Mustaine3]

What is so complicated with *Distribution and *Distribution Table? Read the Analysis Users Guide regarding that topic and look at the examples at the end of that page.

 

[ardalansv]

Hello Mustaine3,

My problem is not with *Distribution or its Table, my concern is that in one of the examples that is written in the documentation as shown below, dist1 is assigned to *Elastic. How is it possible to assign dist1 in CAE in the property section, since when you make an elastic material it is asking for modulus and Poisson's ratio, and you cannot leave them empty. Could you help me solve this? I apologize that it might seem very simple problem for you.

Regards,

*DISTRIBUTION TABLE, NAME=tab1
MODULUS, RATIO
*DISTRIBUTION, NAME=dist1, LOCATION=element, TABLE=tab1
, E0, 0
element set or number, E1, 1
element set or number, E2, 2
…
*MATERIAL, NAME=MAT
*ELASTIC
dist1
*PLASTIC
…
*SOLID SECTION, ELSET=elset3, MATERIAL=MAT

 

[IceBreakerSours]

Click here.

As the old timers might say, RTFM. The solid mechanics documentation for Abaqus is top-notch. If you read it carefully, you will learn.

*********************************************************
Are you new to this forum? If so, please read these FAQs:

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

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[Mustaine3]

I think the distribution for the elasticity cannot be defined in A/CAE. It has to be done in the input file. Or do it in a separate file and link it to the input file with *Include.

 

[ardalansv]

Thank you Mustaine3, you are right it is not possible in CAE and I had to run it through the inp.

Regards,

Ardalan