# Calculix equivalent to Ansys force bonded

**URL:** <https://calculix.discourse.group/t/calculix-equivalent-to-ansys-force-bonded/4108>\
**Category:** Model setup\
**Created:** [September 10, 2026, 7:50am UTC](https://calculix.discourse.group/t/calculix-equivalent-to-ansys-force-bonded/4108 "2026-09-10T07:50:24Z")\
**Posts on this page:** 3\
**Page:** 1

<div class="post-metadata">

**Author:** ![linth](https://avatars.discourse-cdn.com/v4/letter/l/898d66/32.png) [@linth](https://calculix.discourse.group/u/linth)\
**Post date:** [September 10, 2026, 7:50am UTC](https://calculix.discourse.group/t/calculix-equivalent-to-ansys-force-bonded/4108/1 "2026-09-10T07:50:24Z")

</div>

Hi there,

Ansys provides ways to treat contact different in a prestressed modal analysis in different ways:

- true status (e.g. if sliding in static, than only normal contact stiffness is used in the modal analysis, if sticking use both normal + tangential stiffness in modal)
- force bonded (e.g. if in contact (not open), than use both normal and tangential stiffness in modal analysis

From the beamptied4-7 examples I understand that Calculix seems to follow the “true status” way.

Is there a way to get Calculix go the “force bonded” in a perturbed frequency step? Or more general, is there a way to change the contact properties in a perturbed frequency step?

Thanks, Thomas

---

<div class="post-metadata">

**Author:** ![Calc\_em](https://avatars.discourse-cdn.com/v4/letter/c/43a26b/32.png) [@Calc\_em](https://calculix.discourse.group/u/Calc_em)\
**Post date:** [September 10, 2026, 8:41am UTC](https://calculix.discourse.group/t/calculix-equivalent-to-ansys-force-bonded/4108/2 "2026-09-10T08:41:56Z")

</div>

In CalculiX, contact status remains frozen in perturbation (e.g. modal) steps. There are no special settings for that. You can slso use tie constraints. They apply kinematic constraints to permanently bond surfaces, also in modal analyses. But it’s not a contact algorithm.

---

<div class="post-metadata">

**Author:** ![linth](https://avatars.discourse-cdn.com/v4/letter/l/898d66/32.png) [@linth](https://calculix.discourse.group/u/linth)\
**Post date:** [September 15, 2026, 9:57am UTC](https://calculix.discourse.group/t/calculix-equivalent-to-ansys-force-bonded/4108/3 "2026-09-15T09:57:05Z")

</div>

Looks like I found a solution. The keywords CHANGE FRICTION and CHANGE SURFACE BEHAVIOR can be used to change both normal and tangential contact stiffness, even if there was no FRICTION set in the original contact definition. A modal analysis run with a friction coefficient changed from 0 to a large number looks very much like the Ansys “forced bonded”.

\*STEP,PERTURBATION  
\*CHANGE friction,interaction=frictionless  
\*friction  
1e20,1.e7  
\*CHANGE surface behavior,interaction=frictionless  
\*SURFACE BEHAVIOR,PRESSURE-OVERCLOSURE=linear  
1.e20  
\*FREQUENCY  
10  
\*END STEP