Time dependent material propertie (Young's modulus) 2

[franjm]

Hello,

Hello I am doing a thermal analysis of concrete at early ages and I would like to introduce the elastic modulus versus time to take account of cement hydration.

I added in the material properties of a field variable as follows:

*Elastic, dependencies=1
** E, v, temp, FV1
1.89e+10, 0.3, , 86400
2.45e+10, 0.3, , 604800
2.85e+10, 0.3, , 2.42e+6

where PV1 is the time in seconds, which I am not sure it's right. If the above is correct I would like to know how to tell Abaqus FV1 is "time". I am a bit new to Abaqus so grateful if I indicate what I have to use code to do so, since in Abaqus/CAE I think it's not possible.

thank you very much

 

[akabarten]

Hi,

Field variable isn't the time but of course you can change the field variable respect to the time.

** model data section
**
** section definiction
*SOLID SECTION, ELSET=myElset, MATERIAL=myMaterial
**
** material definition
*MATERIAL, NAME=myMaterial
*ELASTIC
**     E,   v, temp, FV1
1.89e+10, 0.3,     , 0.0
2.45e+10, 0.3,     , 1.0
2.85e+10, 0.3,     , 2.0
**
** nset with all nodes with myMaterial
*NSET, NSET=myField-NSET, ELSET=myElset
**
** history section
**
** amplitude to change FV1 during the time
*AMPLITUDE, NAME=myAmp
**   time, FV1 
    86400, 0.0
  6040800, 1.0
 2.42e+06, 2.0
**
** field variable definition
*FIELD, VARIABLE=1, AMPLITUDE=myAmp
myField-NSET, 1.0
**

Short explanation:
First Abaqus sets field variable to all nodes with "myMaterial" material respect to the amplitude.
Next check what FV1 value is in current increment and define correct E respect to a table under *ELASTIC keyword.

Regards,
Bartosz

 

[franjm]

Thank you very much for the code and the explanation Bartosz! They were very helpful.

Now I have another problem. I modify the input file and introduce the code to define the field variable. And when I submit the job, it aborts with this error message:

"in keyword *FIELD, file "myfile.inp", line 2420: The keyword is misplaced. It can be suboption for the following keyword(s)/level(s):step, postoutput. Analysis Input File Processor exited with an error"

I have been reading Abaqus Documentation and I think the problem is that Predefined field variables are not supported in Abaqus/CAE but I don't know what to do to solve it.

Thank you very much,
Fran

 

[akabarten]

Hi Fran,

The error is pointing that *FIELD keyword is in wrong place in an inputdeck.
Abaqus's inputdeck is split into two sections "model data" and "history data".
First is model data and after first *STEP keyword starts history data.
*FIELD keyword has to be pleaced in history data, it means after *STEP keyword.

I think the problem is that Predefined field variables are not supported in Abaqus/CAE

I do not know that, I have almost no experience with Abaqus/CAE.

I don't know what to do to solve it.

You can update your inputdeck in any text editior. This is just ASCII file.
That modification you can also do from Abaqus/CAE: Model --> Edit keywords.

Regards,
Bartosz

 

[franjm]

Thank you very very much for your help Bartosz!

I placed *FIELD keyword in history data (after *STEP keyword) and it works.

Regards,
Fran

 

[themaninblue]

fanjm,

I was trying to model this very thing a few months ago, and similarly had a lot of difficulties capturing the neccessary effects of young hardening concrete in Abaqus.

As suggested, field dependency terms can be used to change the stiffness. However, I was not sure about whether abaqus was producing an accurate result.

If the concrete is under load during cure, it will have a given stress and strain state. If you then change the stiffness of the concrete using field dependency, termperature dependancy or otherwise, either the stress or strain will change to maintain equilibirum (depending whether displacement controlled or load controlled). So if the stiffness increases by a factor of 10, the stress will change by a factor of 10 for constant strain. Try this for yourself on a small model to check.

My understanding is that as new concrete hydrates, the newly cured concrete has a stress state of 0, so the stress and strain of the bulk concrete should not change due to the curing alone (although they may change due to thermal expansion effects or changing loads etc).

I did manage to find a long way around this and can explain, but would be interested to hear if you agree this is the case?

Cheers

Tom

 

[MalibuStone]

Thank you guys....You just simplified my problem after a good 8 hours of struggling. Good logic akabarten. keep up the good work.

 

[donrick]

I am pretty new to ABAQUS and learning from scratch. I am currently trying to model a weld simulation to determine the temperature and stress distribution after cooling. I tried using the heat transfer step to determine the temperature distribution afterwards, but there was no temperature recorded. Could somebody give me a hint on the best way to model the weld and perform the simulation? Thanks.