Often enough when working with contact problems we want to consider the full surface slip between our surfaces – not the directional components CSLIP1 and CSLIP2.

CSLIPEQ represents the total slip length at a slave or edge node while in contact. Incremental contributions to CSLIP1 and CSLIP2 are computed as the scalar product of the incremental relative nodal displacement vector and the respective local tangent direction, t_1 (CTANDIR1) or t_2 (CTANDIR2).

About general contact in Abaqus/Explicit
Figure 1

Previously we either had to perform some script magic or use the “Create Field Output” functionality to compute CSLIPEQ. However, from Abaqus 2019 CSLIPEQ is available as fieldOutputs in both Abaqus /Standard and Abaqus/Explicit. It is not available through the CAE in the FieldOutput dialog – but only as keywords. We will show you how!

Benchmark Model

Our benchmark model is an assembly of two steel cubes of 20x20x20mm which will be squeezed together and then subjected to tangential movement. See figure 1.


Material coefficients
Youngs modulus: 210GPa
Poisson’s ratio:  0.3
Frictional coefficient: 0.2

Mesh
1000 elements per cube, C3D8R elements

Loads and BCs
Over two steps we apply a pressure of 0.05MPa on the cube in step 1, and then we drag the whole top cube 0.2mm in both tangential directions in step 2

How to enable CSLIPEQ

We have add the following CSLIP to the keyword editor under  *Contact Output for each step we want this output from:

NB: Remember to add CSLIPEQ to all steps which you want this output from!

Expectations and Results

From our loads, we expect the following results

  • CPRESS = 0.05MPa (step 1)
  • CSLIP1 and CSLIP2 = 0.2mm (step 2)
  • CSLIPEQ = 0.2828mm

Step 1

Step 1: CPRESS, uniformly 0.05047MPa

Step 2

Step 2: CSLIP1/2 is 0.2mm and CSLIPEQ is 0.2828mm, right on the money!

Our results is pretty much spot on – and we’ve seen that CSLIPEQ can successfully be used in Abaqus 2019 with /Standard!

Thanks for reading! Signing off.