1
$\begingroup$

I am modelling a plate as 3D deformable solid. My plate has a spatially dependent isotropic thermal expansion coefficient.

I have defined this spatial distribution as a Discrete Field in a tabular form (for the mesh elements). My question is how can I link this distribution to my material definition? Or is it not possible to have spatially dependent thermal expansion in Abaqus/CAE?

Thanks!

Improve this question
$\endgroup$
4
  • $\begingroup$ The "standard" data model for FE software is: (1) An element is made from a material (or several materials if it is a layered shell). (2) A material has thermal expansion coefficient(s) that are functions of temperature. I can't see any logical reason why you couldn't have thermal properties that were functions of position (of the undeformed structure) but you would have to rewrite the element routines to do that - so you would end up with pretty much a new FE program for a (presumably) rather specialized application. $\endgroup$
    – alephzero
    Commented Jun 13, 2018 at 19:19
  • $\begingroup$ … I suppose you could write such an element as a "user element," but it's a very long time since I messed with Abaqus at such a low level! $\endgroup$
    – alephzero
    Commented Jun 13, 2018 at 19:22
  • $\begingroup$ Without messing around too much in material subroutines, if your element resolution is fine enough you can define a different thermal expansion coefficient on every element instead. $\endgroup$
    – dROOOze
    Commented Jun 20, 2018 at 12:35
  • $\begingroup$ Thank you for the suggestions. I figured out a simpler way in 2018-Abaqus/CAE and posted the answer. $\endgroup$
    – Tristan S
    Commented Jun 21, 2018 at 14:56

1 Answer 1

Reset to default
0
$\begingroup$

It turns out that defining predefined field variables in CAE is a feature that was added in the 2018 version. The steps that one needs to follow when creating a field-dependent material property are the following:

1) In the Property module, make your Material dependent on a Field Variable(s) by specifying the number of field variables. In the table you will have to map the material property to the field variable.

2) Create the Field Variable: In the Load module, go to "Predefined fields"->Create->Other->Field and specify the desired distribution, which can be one of several options, including an Analytical Field. This analytical field in my case is the spatial distribution of the expansion coefficient - a function of X,Y,Z.

In case you have an earlier version of Abaqus/CAE, apparently you could use a temperature definition for the Field, and modify your input file to reroute to the field variable. I haven't tried this approach, but it should work just as well.

A couple people suggested parts of this and then I finally figured the rest out through some trial and error. Thanks!

Improve this answer
$\endgroup$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.