D is for “Ductile Damage”

The FEA dictionary is back and it’s time for letter D! Today I will introduce you to one of the methods to introduce damage in your material models.

Although it was created based on the failure of metals, this damage model can be used to introduce the degradation of mechanical properties for other types of materials. This option is available in Abaqus/Standard and Abaqus/Explicit and it requires the definition of the ideal elastic-plastic behaviour of the material, a damage initiation criterion and a damage evolution response. Please note that if any of the requirements cited before is not defined, the material properties will not be degraded.

In Abaqus there are different options for the damage initiation criterion and basically they can be classified as follows:

  • Criteria for fracture of metals (ductile and shear).
  • Criteria for necking of sheet metal.

All of these initiation criteria use a variable to indicate whether the criterion has been met (value greater than or equal to 1) or not (value less than 1). It has to be said that more than one initiation criteria can be used for the same material that we are modelling and they will be treated independently. In Abaqus, it can only be used in conjunction with Mises, Johnson-Cook, Hill and Drucker-Prager plasticity. Out of all the initiation criteria, the simplest one is the so called “ductile criterion”. This model assumes that the equivalent plastic strain when failure occurs is a function of stress triaxiality and strain rate:


The stress triaxiality is equal to the pressure stress over the von Mises stress. Hence, for defining our criterion, we need to specify three rows of properties:

  • Uniaxial compression: a value of  the plastic strain at which failure occurs; the stress triaxiality for this particular case (equal to -0.32); strain rate.
  • Pure shear: a value of the plastic strain at which failure occurs; the stress triaxiality for this particular case (equal to 0); strain rate.
  • Uniaxial tension: a value for the plastic strain at which failure occurs; the stress triaxiality for this particular case (equal to 0.32); strain rate.

If we wanted to get rid of the strain rate dependency, we would only have to input the same value for all cases. Then, the failure variable which was introduced before, is calculated as follows:


In order to check the failure variable, it is important to request the Field Output DUCTCRT… The only problem is that it is impossible to find that variable in Abaqus CAE. So, how do we request it? Pretty easy, just tick the DMICRT box in the Failure/Fracture menu and your desired variable will appear once the simulation is completed!

Apart from the initiation criterion, we also need to include the damage evolution law. Basically, it introduces the rate of degradation of the material stiffness once the corresponding initiation criterion has been satisfied. Abaqus uses a variable (D) to model this progressive damage. When the failure has not occurred, the damage variable remains equal to zero. However, once the criterion is met, the damage variable starts to increase, being 1 its maximum value. In other words, the material is fully damaged once this variable reaches 1. Then, Abaqus recalculates the stress of every element using the following the expression which is introduced below. In order to check the value of the variable in the results, we need to request the Field Output SDEG, under the Failure/Fracture menu.


The evolution of damage can be introduced in tabular, linear or exponential form. Depending on the experimental data or information that you’ve got, you will use one or another.

A representation of the typical response of a material which has been defined correctly is presented below, where the dashed curve represents the ideal behaviour (i.e. with no failure):


Ductile damage response (source: Abaqus Documentation)

Also, the user has control over element deletion for this damage model. By default, the elements will be deleted once the damage variable reaches 1. However, that value can be modified in the mesh module, so that it can be deleted for a lower value or not deleted at all.

To sum up, let me summarise the steps that you should follow to use this damage model:

  1. In the Property module, create a new material.
  2. Go to Mechanical, Elasticity, Elastic and define the properties.
  3. Go to  Mechanical, Damage for Ductile Metals, Ductile Damage and define the initiation criterion (including the three rows for uniaxial compression, pure shear and uniaxial tension).
  4. Click on Suboptions and select Damage Evolution to specify the way the damage variable will behave.
  5. Go to the Step module, and click on  Field Output. Then, expand the Failure/Fracture menu and tick SDEG and DMICRT.
  6. Go to the Mesh module, click on Assign Element Type and then specify the Max Degradation that you want.

I really hope that this post will help some of you guys! While I prepare the new FEA Dictionary post, I will also post other content on the blog so don’t get very anxious! Take care!

2 thoughts on “D is for “Ductile Damage”

  1. Salar

    Thanks for the great explanation above. I don’t, however, understand the part where DUCTCRT is calculated. You define a tabular data (3 rows) on Equivalent Fracture strain, strain triaxiality and strain rate. that’s fine. How does the integration work? I dont understand the difference between the denominator and numerator.
    There are two stress triaxialities here:
    1. is defined in the ductile damage model (material property module)
    2. is obtained during the stress analysis for each increment, the ratio of hydrostatic pressure to Von Mises equivalent stress.
    I’m confused how these two are related.


    1. Ignacio Carranza Guisado Post author

      Hi Salar, thank you for your comment. From the official documentation it is not clear at all! But based on my experience, what Abaqus does is to recreate some kind of failure envelope in the hydrostatic pressure – von Mises stress space (p-q space). That envelope is recreated by fitting the experimental data defined in the material property module (in this case the typical values are uniaxial compression, uniaxial tension and pure shear). Hence, at each increment it evaluates the stresses in each element and correlates it to that “envelope”. Ideally, we could define a fairly accurate failure envelope by using the Arcan test to study different mixed mode loading conditions, which would allow us to get several relationships between von Mises and hydrostatic pressure.

      I think I’m not explaining myself very well here (sorry about that!), but there is a bit more information regarding this p-q space in the Abaqus Documentation section about the “Crushable Foam” material model, which does something similar to create the yield surface of the material.

      I’ll try to look into this a bit more in detail! Thanks!



Leave a Reply to Ignacio Carranza Guisado Cancel reply

Fill in your details below or click an icon to log in:

WordPress.com Logo

You are commenting using your WordPress.com account. Log Out /  Change )

Google photo

You are commenting using your Google account. Log Out /  Change )

Twitter picture

You are commenting using your Twitter account. Log Out /  Change )

Facebook photo

You are commenting using your Facebook account. Log Out /  Change )

Connecting to %s