My model is unstable. What could be the reason?


There can be various reasons for the calculation abort due to an unstable structural system. On the one hand, it can indicate a "real" instability due to overloading the structural system, but on the other hand, the modeling inaccuracies may also be responsible for this error message. In the following, you find possible procedures to find the instability cause.

1. Check of Modeling

First, you should check if the modeling of the structural system is all right. It is recommended to use the model check tools provided by RFEM/RSTAB [Tools → Model Check]. For example, these options allow you to find identical nodes and overlapping members, so you can delete them, if necessary.

Furthermore, the structure subjected to pure dead load can be calculated in one load case according to the geometrically linear analysis, for example. If results are displayed subsequently, the structure regarding the modeling is stable. If this is not the case, the most common causes are listed below (see also the video "Model Check" under "Downloads"):

  • Incorrect definition of supports / lack of supports
    This can lead to instabilities as the structure is not supported in all directions. Therefore, the support conditions must be in equilibrium with the structural system as well as with the external boundary conditions. Statically overdetermined or kinematic systems may also lead to calculation aborts due to a lack of boundary conditions.

    Figure 02 - Kinematic System - Single-Span Beam Without Rigid Support

  • Torsion of members about their own axis
    If members rotate about their own axis, that is, a member is not supported about its own axis, it can lead to instabilities. This is often caused by the settings of member hinges. Thus, it may happen that there are the torsional releases entered at both the start node and the end node. However, you should pay attention to the warning that appears when starting the calculation.

    Figure 03 - Entering Torsional Releases on Start and End Nodes

  • Missing connection of members
    Especially in the case of large and complex models, it may quickly happen that some members are not connected to each other, and thus they "float in the air." Also, if you forget about crossing members that should intersect with each other, it can lead to instabilities as well. A solution provides the model check of "Crossing Unconnected Members," which searches for the members that cross each other, but do not have a common node at the intersection point.

    Figure 04 - Result of Model Check for Crossing Members

  • No common node
    The nodes rest apparently at the same location, but on closer inspection, they deviate slightly from each other. This is often caused by CAD imports, and you can correct it by using the model check.

    Figure 05 - Result of Model Check for Identical Nodes

  • Formation of hinge chain
    Too many member hinges at a node may cause a hinge chain, which can lead to the calculation abort. For each node, you can only define n‑1 hinges with the same degree of freedom with regard to the global coordinate system, where "n" is the number of the connected members. The same applies to line releases.

    Figure 06 - Kinematic System due to Hinge Chain

2. Check of Stiffening

If the stiffening is missing, it may also lead to the calculation aborts due to instabilities. Therefore, you should always check whether the structure is stiffened sufficiently in all directions.

3. Numerical Problems

An example of this is shown in Figure 08. It is a hinged frame that is stiffened by tension members. Because of the column contractions due to vertical loads, the tension members receive small compressive forces in the first calculation step. They are removed from the structure (since only tension can be absorbed). In the second calculation step, the model without these tension members is unstable. There are several ways to solve this problem. You can apply a prestress (member load) to the tension members in order to "eliminate" the small compressive forces, assign small stiffness to the members, or remove the members one by one in the calculation (see Figure 08).

4. Detecting Causes of Instability

  • Automatic model check with graphical result display
    In order to obtain a graphical display of the instability cause, you can use the RF‑STABILITY (RFEM) add-on module. Select the "Calculate eigenvector for unstable model…" (see Figure 09), it is possible to calculate the unstable structure. The eigenvalue analysis is performed on the basis of the structural data so that the instability of the affected structural component is displayed graphically as a result.

    Figure 09 - Graphical Display of Instability

  • Critical load problem
    If load cases or load combinations are calculated according to the geometrically linear analysis, and the calculation is only aborted as of the second-order analysis, there is a stability problem (critical load factor less than 1.00). The critical load factor indicated which coefficient must be used to multiply the load so that the model subjected to a specific load becomes unstable (for example, buckling). Therefore: The critical load factor of less than 1.00 means that the system is unstable. Only the positive critical load factor greater than 1.00 allows for the statement that the loading due to the specified axial forces multiplied by this factor leads to the buckling failure of a stable structure. In order to find the "weak point," the following approach is recommended, which requires the RF‑STABILITY (RFEM) or RSBUCK (RSTAB) add-on module (see also the video "Critical Load Problem" under "Downloads").

    First, it is necessary to reduce the load of the affected load combination until the load combination becomes stable. The load factor in the calculation parameters of the load combination can help. This also corresponds to the manual determination of the critical load factor if the RF-STABILITY or RSBUCK add-on module is not available. In the case of pure linear structural elements, it may already be sufficient to calculate the load combination according to the geometrically linear analysis and select this directly in the add-on module. Then, the buckling curve or shape can be calculated and displayed graphically on the basis of this load combination in the corresponding add-on module. The graphical result display allows you to find the "weak point" in the structure and then optimize it specifically. By default, the RF-STABILITY or RSBUCK add-on modules only determine global mode shapes. In order to also determine the local mode shapes, it is necessary to activate the member division (RF‑STABILITY), or to increase the division for trusses to "2" at least (RSBUCK).

    Figure 10 - Activating Division for Members in RF-STABILITY

    Figure 11 - Member Division in RSBUCK


Instability System unstable Structure unstable Singularity Instability cause



Contact us

Contact to Dlubal

Did you find your question?
If not, contact us via our free e-mail, chat, or forum support, or send us your question via the online form.

+49 9673 9203 0

RFEM Main Program
RFEM 5.xx

Main Program

Structural engineering software for finite element analysis (FEA) of planar and spatial structural systems consisting of plates, walls, shells, members (beams), solids and contact elements

Price of First License
3,540.00 USD
RSTAB Main Program
RSTAB 8.xx

Main Program

The structural engineering software for design of frame, beam and truss structures, performing linear and nonlinear calculations of internal forces, deformations, and support reactions

Price of First License
2,550.00 USD