For a bonded contact, which is the default for models opened in Ansys Workbench Mechanical, the contacts are modeled using elements TARGE170 and CONTA174. The thermal conductivity and stiffness of the contact elements are calculated by Ansys based on the properties of the two bodies. The controls only allow one to change the contact stiffness factor FKN which is a multiplier but not the actual stiffness of the joint (ie with SI units of N/m/m^2). However if one would like to set the value of the contact stiffness or thermal contact resistance, it can be done using Command snippets (also known as the Commands Object) for each contact. Using the commands object, one can set the joint’s normal stiffness FKN, tangential stiffness FKT, and thermal contact conductance TCC (in SI units W/m^2-K).  One can also change a keyopt to set the units of the contact’s stiffness as Force divided by displacement (SI units of N/m) and specify the stiffness value that way.

Below is a simple example with rectangular solid bars in contact.  All bodies are “structural steel”.  The long connecting bar between the two blocks has dimensions 100 mm long x 10 mm high x 20 mm deep.  The left end if fixed.  A force of 1000 N is applied to the block at the right.

MECHANICAL CONTACT STIFFNESS

We show how to change both the normal and shear or lateral contact stiffness.  Either or both stiffness values can be specified.

Without changing the default behavior, the distortion picture due to an axial force is

Without modifying the default stiffness behavior, the distortion due to a lateral force is

Now we insert a command snippet

Within the snippet, we use the following commands to specify the normal and lateral contact stiffness.  We also need to change the formulation of the contact area to be Pure Penalty.  The Pure Penalty contact formulation uses force =stiffness*penetration, where the penetration is the separation between bodies.  The pure penalty setting can be specified either under the details of the contact of interest or in the command snippet by changing a keyopt or both.

Below is the command snippet.  The units of the connection’s contact stiffness are stiffness per area, or N/m/m^2 in SI units.  The negative sign is required to treat the number as a stiffness value instead of a multiplication factor of its own contact stiffness calculation (below we also show how to change a keyopt to specify the contact stiffness in units of force/displacement or N/m in SI units).

KEYOPT,CID,2,1        !Pure penalty contact stiffness formulation by setting KEYOPT(2)=1
RMODIF,TID,3,-1e11    !normal stiffness N/m/m^2
RMODIF,TID,12,-1e-10  !shear stiffness N/m/m^2

Using the command snippet, the distortion due to a normal force is

The normal contact stiffness is k=1e11 N/m^3 x 20mm x 10mm= 20e6 N/m.  A 1000 N normal force results in a normal displacement of x=F/k=50 um.  The FEA result of 53 um is due to the additional stretching of the long bar.

Using the command snippet, the distortion due to a transverse force is

The shear contact stiffness is k=1e10 N/m^3 x 20mm x 10mm= 2e6 N/m.  A 1000 N lateral force results in displacement of x=F/k=500 um.  The FEA results of 1.56 mm is due to the additional bending of the long bar.  The reduced normal stiffness also contributes as it changes allows for rotation between the block and bar.

As mentioned above, we can also change a keyopt allow specification of the contact stiffness value using units of force/displacement as shown in the snippet below.  Again the value must include a negative sign to work correctly.

KEYOPT,CID,2,1        !Pure penalty contact stiffness formulation by setting KEYOPT(2)=1
KEYOPT,CID,3,1        !Set units of contact stiffness to be force/displacement by setting KEYOPT(3)=1
RMODIF,TID,3,-20e6    !normal stiffness N/m
RMODIF,TID,12,-2e6    !shear stiffness N/m

THERMAL CONTACT RESISTANCE

Next, we examine a steady state thermal problem for the same geometry of the two blocks connected by a bar.

We place a temperature condition on each end such that the temperature varies along the length of the blocks. By changing the thermal contact resistance we should see changes in the gradient.

With the default thermal contact resistance, we see a most of the gradient along the length of the bar.

Now we insert a command snippet to change the contact at the right side of the bar.

 

RMODIF,TID,14,1E-6  !Thermal contact conductance W/m^2-K

Using the command snippet, we made the thermal contact resistance very large by setting the value of thermal contact conductance (TCC) small, 1E-6 W/m^2-K in this case.  Then, we re-run the simulation and see that the temperature gradient is almost entirely at the contact.   The thermal resistance of the contact is R=1/(1E-6 W/m^2-K x 20 mm x 10 mm)=5E9 K/W