Understanding Contact Reaction Probes in ANSYS Mechanical

contact reaction probesThere are three methods available for extracting the reaction forces across a contact region in WB-Mechanical:

  1. Contact(Underlying Element)
  2. Contact (Contact Element)
  3. Target (Underlying Element)

When you choose ‘Contact(Underlying Element)’, the code is selecting the contact elements associated with that region, selecting nodes attached to the selected contact,  and then selecting elements attached to the selected nodes before calculating the reaction.

Below is an equivalent APDL command script, where “cid1″ is a parameterized contact element type number for the region of interest.


When you choose ‘Contact (Contact Element)’, the code is only selecting the contact elements and executing “NFORCE,cont”

Below is an equivalent APDL command script.


The ‘Target (Underlying Element)’ option is similar to the first except we select the Target elements (Type=tid1) instead of the contact elements. Below is an equivalent APDL command script.


The availability of these reaction options is governed by the MISC option of the OUTRES command.

(Refer to on-line documentation:  // Mechanical User Guide // Using Results // Structural Results // Structural Probes // Reactions: Forces and Moments for more details.)

Often all three methods produce the same calculated reaction.

Sometimes they will not agree because either the contact and/or the target surfaces share nodes with other constraints or other contact regions.

When this happens, one or more of the methods will calculate a force summation that represents the load transmitted across the contact region in question plus other loads from other sources. The overall result of the FEA model is not necessarily wrong, but these probed force calculations are no longer representing only the load across the contact region of interest. The first suggested workaround is to try to employ a strategically tighter trim tolerance to eliminate this unwanted force bleed off. Trim will remove both contact and target elements from respective surfaces that are separated by a distance larger than the user defined tolerance. In some cases, the default tolerance might be too large or perhaps Trim technology is turned off altogether.

Note, for Trim contact set to “Program Controlled”, it will be off for manually created pairs and if large deflection is ON (for models created in R14.5). If Trim options are not successful or not practical, you might need to consider a change to the way the model is constrained or a change in the contact regions definitions.

What happens if there are no shared constraints and the ‘Contact (Contact Element)’ option does not agree with the other two? The question to ask in this circumstance — Is this problem being run as small deflection with linear contact? If so, does the contact pressure profile look reasonable for the given load?  If it does not look reasonable or you are not sure, try turning on large deflection and re-running the analysis. It is important to understand that the ‘Contact (Contact Element)’ extraction option is using the contact pressure profile integrate over the contact surface to calculate the overall reaction force.   Hence, this calculation is only as accurate as the accuracy of contact pressure profile. If it is not really a large deflection application and you are not interested in running multiple  iterations to improve the contact pressure profile, you could switch to MPC formulation.  This will block the ‘Contact (Contact Element)’extraction method altogether.

10 thoughts on “Understanding Contact Reaction Probes in ANSYS Mechanical

  1. how to model a contact between a 8node shell element and a 3 node beam element using multipoint constraints method will you please tell me the procedure to do the model .

  2. Hi Anupama:

    You can use a face-to-edge contact pair to do this. It will work with higher order or lower order elements. Scope the edge (meshed with higher order beams) as the contact and the surface (meshed with higher order shells) as the target. If it seems like it is over constrained, try the contraint type “Target Normal, uncoupled U to ROT”. MPC formulation will only support bonded and no-separation contact. If you are trying to model nonlinear contact (frictional, frictionless or rough), than you have to use a penalty based formulation.


  3. Tell me more thing about doing contact non-linear problem in ansys workbench for cold hole expansion project.

    • Hi Prashant:

      I am not familiar with “cold hole expansion project”. Do you have a specific contact question or concern as it relates to this project?


  4. Hi, John Doyle,
    I am now doing a frictional contact simulation, it is a simplified 2D model. I try to use “force reaction” to get the frictional force between the contact and target surfaces (there is relatively sliding between these two surfaces). Should I get the normal force from total force reaction and then multiply by the frictional coefficient, or just get the tangential component of the force reaction?
    I found two questions in the result:
    1. The tangential component of the force reaction is not equal to normal force multiplied by frictional coefficient. Should they be equal to each other if the tangential component of the force reaction is frictional force?
    2. The normal force extracted from contact surface is a little different from that extracted from target surface. Why?
    Can you tell me why, and how to extract the friction force between them correctly?

  5. Xiaoxiao:

    Could you orient the reaction probe to a user defined coordinate system such that X is strategically oriented along the tangential direction and Y is oriented normal to the surface? Of course this would only be helpful to you if the contacting surfaces are flat.

    I think Ft=mu*Fn would only match the probe reaction if all the contact status are consistent and the force distribution is uniform across the surface.

    Do any of the suggestions in the blog help explain the differences between target and contact reactions?

    • Hi, John Doyle,
      Sorry for my late reply.

      Yes, in my simulation, X is strategically oriented along the tangential direction and Y is oriented normal to the surface, and the contacting surfaces are all flat when they contact with each other.

      Also, large deflection is on. The contact surface and target surface do not share the elements with each other, as there is a sliding motion between them.

      What do you mean “all the contact status are consistent”?

      Best regards,


      • I was referring to the fact that for contact elements that are closed and sticking, the reaction might be less then mu*fn. For elements that are closed and sliding the reaction will be mu*fn but no more.

  6. Hi John
    I have layered shell181+solid185 element structural model that I solve under a static force. It calculates the reaction forces for any constrained node. What do I need to do to get the internal nodal reaction forces at unconstrained shell (181) and solid185 nodes?

Comments are closed.