I revisited this dogbone necking project in Nov, 2020.  My main goal was to reduce the mesh size and repeat the calibration to get a sense of overall run times.  This mesh is 5x10x30 (width x height x length) = 1500 elements. 
The 1500 C3D8R mesh/model takes ~13 seconds to run on 1cpu (laptop). Using 2 or 4 cpus does not speed it up. I also realized that I had not kept track of units issues in the larger model. This titanium dogbone specimen was originally set up in English units of inches, lbf, and psi.

Dogbone specimen dimensions in the center region:

Length = 1 inch (extensometer dimension)
Width = 0.123 inch
Height= 0.247444 inch
Area  = 0.0304 inch^2

Nominal Stress = RF/Area = Scale Factor * RF   (where the scale factor = 1/Area = 32.85625)

When we use the calibration app, we can select what units we want to use for the FE runs, and we should make this consistent with the model we have prepared.   Also, it is rather common that engineers prefer to think in terms of nominal stress-strain, since they often have an intuitive sense of the materials stress-strain curve (rather than think in terms of force-disp).  In the demo video below, we output the RF1 in lbf from the FE model, but convert it to nominal stress by the scale factor of 32.856. 

General set of steps:

1) Import the test data as "generic".  Columns of data imported are time, nom stress (psi), nom strain.

2) Import one or more FE mesh/models.

3) Map the FE output of RF1 to be compared to the nominal stress data set.  Set scale factor to 32.85625

4) Select the Johnson Cook elastic-plastic material model.

5) Set E, A, B and n to some reasonable values. Modulus of titanium is ~ 1e5 MPa, or 15e6 psi

6) Use the "Evaluate" feature to show a one-time comparison using the current model parameters.  Possibly adjust parameters by hand and re-run "Evaluate".

7) Run the calibration.

The mapping of the RF1 model output to the test data looks like this:

The demo video below was created on Nov 18, 2020 using a development version of the app. This should be fairly close to the look & feel of R2021x FD05 as it is released in the spring of 2021.  The video does a first calibration without using any min & max bounds. Then a second calibration is performed with most of the min & max bounds set.  There was not a noticeable difference between the two run times.

In the video, I commented that the optimization settings (especially those related to stopping the optimizer) were developed for the very fast running analytical mode.  In the future we may develop a separate set of settings for FE mode, but for now we have not.  This means that manually stopping the optimizer might be quite common in FE mode.  The image below shows the final state of the calibration:

Since we used synthetic test data, we know the right answer. Just to double check things, I then typed in the known right answer.  You see below that the right answer gives a R2 value of a perfect 1 (to 8 decimal places).

Here is a 3dxml file and .inp file that you could download and use:
 

Back to:  Necking of a titanium dogbone specimen

Back to:  FE-based Material Model Calibration

Back to:  Calibration New Features in R2021x FD05

Back to:  New Material Model Calibration App in 3DEXPERIENCE Platform

Back to:  Material Modeling and Calibration - An Overview and Curriculum