# Thread: Converting experimental stress-strain data

1. Junior Member
Join Date
2010-11
Posts
10

## Converting experimental stress-strain data

Hi all,

I wish to perform an analysis on a hyperelastic material in ABAQUS. Reading the manual I discovered that nominal (engineering) stress / strain data is required for defining a hyperelastic material model.

The experimental data I have is presented as Cauchy stress vs. stretch. From my understanding of mechanics Cauchy stress is True stress, is this correct?

Also, I was wondering if it is acceptable to convert Cauchy stress to nominal stress by rearranging the equation given in the plasticity section of the ABAQUS manual, ie:

s_true = s_nom * (1 + e_nom) where [s = stress, e = strain]

Any insight would be greatly appreciated!

Regards,
Dave

2. 1) Yes, Cauchy Stress = True Stress
2) Yes, your equation is correct (it assumes constant volume)

-Jorgen

3. Junior Member
Join Date
2010-11
Posts
10
Hi Jorgen,

Thanks for the reply. I have one more problem, however.

In ABAQUS/CAE I can input my uniaxial experimental data and create a nearly incompressible material model by specifying a Poisson's ratio of 0.49. I can then fit a 3rd Order Ogden function to the eqperimental data. When I use the Evaluate tool in ABAQUS CAE it shows that my material model is stable for all strain increments between -0.5 and 0.5 in uniaxial tension. The plots of the numerical stress/strain and experimental stress/strain for uniaxial tension are in good agreement.

http://files.engineering.com/getfile...c0&file=02.bmp

As a further validation I am trying to perform a single-element uniaxial tension test. I take a single element of unit length/width/depth and constrain particular nodes as shown in the verification manual for ABAQUS. I then apply a fixed displacement to the nodes on the upper face to simulate the tension test. Upon completion I sum the reaction forces at the displaced nodes and plot against their displacement to obtain nominal stress/strain. However when I compare the numerically predicted nominal stress/strain to experimental stress/strain there is a discrepency:

http://files.engineering.com/getfile...7e&file=01.bmp

Any input as to what I'm doing wrong would be greatly appreciated!!

Many thanks,
Dave
Last edited by Dave442; 2011-04-22 at 10:59.

4. My guess is that you are calculating the stress incorrectly from the reaction force
Are you sure you are using the right BC and area?

-Jorgen

5. Junior Member
Join Date
2010-11
Posts
10
Hi Jorgen,

Im pretty sure the problem lies in how I am post-processing the results as when I use the "Evaluate Material" option in ABAQUS/CAE it shows an almost exact agreement bwtween experimental and numerical nominal stress/strain in uniaxial tension.

I have created and constrained an element (C3D8R) in the same fashion as the examples in the verification manual. Nodes on one face are constrained in U1, nodes on another face are constrained in U2 and nodes on the bottom face are constrained in U3. Also, one node at the origin is constrained in U1/U2/U3. I apply a fixed nodal displacement (U3 direction) to the nodes on the top face of the element.

To calculate nominal stress vs nominal strain I sum the RF3 values at the displaced nodes and plot against the U3 values at these nodes. As the element is of unit length / width / depth I shouldn't need to divide these variables by the initial area (Ao=1x1=1) or initial length (lo=1)? Thats ok i think.

When I compare the numerical data to the experimental data I notice that the discrepency between the results increases as the strain increases? I have attached a copy of my input file if anyone cares to glance at it. I am working in ABAQUS/Explicit.

Many thanks,
Dave

6. Junior Member
Join Date
2010-11
Posts
10
Hi all,

I figured out my issue. I should have mentioned that I have defined this material model in ABAQUS/Explicit and having no compression data I specified a Poisson's ratio of 0.49 when fitting the strain-energy function.

When I re-run the analysis with a Poisson's ratio of 0.499 and 0.4999 I get much closer results from the single element test though I do encounter warning messages about the size of the compression parameter d1 in the strain energy function. This issue is discussed in the ABAQUS manual and from my understanding it appears that a trade-off is required between stress-strain accuracy and numerical stability with nearly incompressible materials in the Explicit solver.

Despite the warning messages I mentioned my models appear to be solving just fine with higher Poissons ratio so far. If anyone has any advice on this issue I would be happy to hear it though.

Thanks again,
Dave

#### Posting Permissions

• You may not post new threads
• You may not post replies
• You may not post attachments
• You may not edit your posts
•