UMAT anisotropic elasto-plastic material

[ar_chatt]

Thanks for the reply everyone.

Yes this is a special kind of steel and i have no more data other than the one mentioned.

Also, with
*ELASTIC 210000,0.3
*PLASTIC
10,-100.0
10,-0.000000001
350,0.000000001
350,100.0

firstly, ABAQUS gives the plastic strain at first must be zero. Secondly, if I draw the stress-strain curve with the mentioned input then it do not represent exactly the same curve that I am supposed to represent (i.e. instead of having both stress and strain negative in compression, the input data will indicate negative strain only).

Thanks.

[matsgd]

Yes, that won't work. Here's why: The *PLASTIC assumes that plastic flow is incompressible, i.e. plastic volumetric strains remain zero, and the plastic behavior only depends on the deviatoric part of the stress tensor, and more specifically on the (scalar, invariant) von Mises stress. Under these assumptions, the plastic behavior is characterized by a hardening curve, relating flow (current yield) stress to equivalent plastic strain. The equivalent (effective) plastic strain is by definition non-negative. So, you need to ask yourself what you mean by "different in tension and compression". If you think about a uniaxial "test", in which you pull the material under the stress +sigma, and then compress the material under the stress -sigma, the *effective* von Mises stress is still just sigma... What's different then? Well, the hydrostatic stress goes from +sigma/3 to -sigma/3. This is why I suggested using a constitutive model with pressure dependence.

But I am sensing something else might enter into this story. What are the typical strain levels that you consider?


Mats

Thanks for the reply everyone.

Yes this is a special kind of steel and i have no more data other than the one mentioned.

Also, with
*ELASTIC 210000,0.3
*PLASTIC
10,-100.0
10,-0.000000001
350,0.000000001
350,100.0

firstly, ABAQUS gives the plastic strain at first must be zero. Secondly, if I draw the stress-strain curve with the mentioned input then it do not represent exactly the same curve that I am supposed to represent (i.e. instead of having both stress and strain negative in compression, the input data will indicate negative strain only).

Thanks.

[Frank]

Here is what I found in my stuff:

"Bilinear cable-like behaviour

One can use element superposition to do this:

1) Create two materials: a) one with *NO COMPRESSION and specifying tension
modulus, and b) one with *NO TENSION and specifying compression modulus

2) Copy the existing set of elements to a new set using *elcopy. Assign the
tension property to the existing set of elements and the compression
material property to the new 'superimposed' elements ('superimposed' because
they share the same nodes).

The element set will now have different properties in tension and
compression."

Note: I did not try this, no warranty is given. You have to replace the NO TENSION and the NO COMPRESSION materials with different elastic-plastic behavior.

Frank

[ar_chatt]

Thanks for the reply...I triel with seveal material models available in Abaqus noting seems to have worked. also, I am not concerned with the amount of strain. I am interested in a perfectly elastic-plastic material i.e. the material stops carrying further load once it has reached elastic limit.

[ar_chatt]

Further,
*NO TENSION and *NO COMPRESSION can carry out the work only if it allows elastic-plastic material behaviour. *NO TENSION and *NO COMPRESSION is restricted to elastic material only, which do not serve my purpose.


Thanks all for your comments.

[lumpwood]

If you are comfortable with using subroutines it would be quite straightforward to write a USDFLD that puts thresholds on load carrying capacity once say a critical principal stress is reached.

[Frank]

You have to replace the NO TENSION and the NO COMPRESSION materials with different elastic-plastic behavior.

[ar_chatt]

Thanks for the reply.
I was thinking about using subroutine. But I am not very conversant with use of subroutine. Can you please help a little more in what to write in USDFLD subroutine. I have used DISP subroutine before.

Thanks everyone.

[lumpwood]

Sorry for delay getting back on this. I don't have enough time to go through a USDFLD in detail but here are some ideas: (bear in mind I've never tried to do exactly what you are doing before).

Create a material with yield stress depending on the value of a field variable (say 350 when the variable is 0 and 10 when the variable is 1).

Use a USDFLD subroutine very similar to the example subroutine in the Abaqus Subroutine Manual to determine min principal stress. If the min stress is lower than yield in compression then use the subroutine to set the field variable to 1.

I've no idea how physical the resulting behavior would be but this should produce different yield behaviors as required. Just bear in mind that USDFLD results in an essentially 'explicit' solution so be careful with time increment size before yield.

[ar_chatt]

Thanks for your reply. This is exactly how I have been trying. I will get back to you if I face some additional difficulty later.