Do you people like Karamba3d? I like it very much and use it a lot.

Karamba3d is a structural analysis plug-in that runs in the Rhinoceros node editor "Grasshopper".
The plug-in is closely tied to the modeling functionality of Rhinoceros, so it can parametrically create complex geometries and perform structural analysis directly within the software, which is a very strong feature of this structural analysis software.

The official website has a fairly extensive collection of example files, which can be very helpful as a reference if you want to perform an analysis using Karamba3d but don't know how to do it.

One of the main concerns with analysis software is the performance of the analysis, and since Karamba3d is not a well-known commercial CAE software like Ansys, for example, we are concerned about the accuracy of the analysis.
However, since this kind of information is not often available, this article will check it for a simple model.

Subject of comparison

Compare Karamba3d's Beam and Shell elements with Ansys' Shell and Solid elements.

Modeling

The analysis is performed with parameters aligned as much as possible so that only solver differences can be identified.

Parameters

• Young's modulus: \(2.0×10^5 \textrm{N/mm}^2\)
• Poisson's ratio: 0.3
• Length: 10.0 mm
• Density: \(7.85 \textrm{g/cm}^3\)
• Mesh size: Meshing to be about 0.25 mm, beam elements also divided about 0.25 mm
• Cross section: 1mm × 1mm rectangle
  • A rectangular cross-section is given for beams, and a thickness of 1mm for shells.

The meshes used are as follows: Ansys can also use quad elements, but Karamba3d can only handle triangles, so to keep the conditions consistent, only triangles are used for comparison.

Comparison Patterns

The following 8 patterns are used to perform the analysis and compare the results.

• Karamba3d
  1. Beam element (KrBe)
  2. Shell element In-plane bending (KrSh-in)
  3. Shell element out-of-plane bending (KrSh-out)
• Ansys
  1. Shell element in-plane bending 1st order element (AnSh1-in)
  2. Shell element in-plane bending 2nd order element (AnSh2-in)
  3. Shell element out-of-plane bending 1st order element (AnSh1-out)
  4. Shell element out-of-plane bending 2nd order element (AnSh2-out)
  5. Solid element Hexahedron 2nd order element (AnSol)

Cantilevered beam tip load

Now we will actually perform the analysis.

Boundary conditions

We will solve the following problem for a cantilevered beam with a fixed base end and a load applied at the tip.

Measuring analysis time

Since Karamba3d is known for its high analysis speed, we will also check the analysis time so that we can compare that as well.

The following values are used for analysis time.

• Ansys analysis time: "Elapsed time spent computing solution" value
• Karamba3d analysis time: Elapsed time spent processing the components of the analysis
  • Analyze(Karamba3D) for linear analysis

Linear static analysis

The predicted value is obtained by the following equation.
The value of the load \(P\) is set to 500N.

\(\delta = \frac{PL^3}{3EI}, \quad
\sigma = \frac{M}{Z}\)

Analysis Results

The results of the analysis are as follows

Karamba3d's Shell element is classified as a 1st order element, and the results show that it has the same level of accuracy as Ansys' 1st order element, but not as accurate as the 2nd order element.

The calculation time is not compared in detail because the Ansys display is limited to 1/10th of a second, but Karamba3d is faster than Ansys.

The numbers in the table are rounded for readability, but the ratios are calculated using the number of digits obtained from the actual analysis.

Large Deformation Analysis

Next, we will perform a large deformation analysis using Analyze Nonlinear WIP in Karamba3d.
The boundary conditions such as load are the same.
The only difference is that the solver used is a large-form solver.

Analysis Results

Since predictions were not calculated for large deformations, the percentages in the table show the difference from the results of Ansys solid elements.

Torsional Load

Now that we have reviewed the bending of cantilevered beams, we will now review the results when a torsional moment is applied to the end of the beam.

Boundary conditions

Set the torsion load to the tip of the beam as follows.

Karamba3d has moment loading on nodes, but it does not have the ability to set rigid connections or MPC for multiple nodes at the tip and apply moment to the center node.

Therefore, when applying a torsional load to a Karamba3d shell element, a rigid beam element is set at the tip and the moment is applied to the center of the beam element so that the tip twists uniformly.

For the Ansys model, MPC is set up and the moment is applied to the center of the cross section.

The value of the load is set to 20 Nmm.

Analysis Results

The results are as follows.

From this we can see that the Karamba3d shell element is torsionally stiffer.
The analysis time was omitted because it is a linear analysis and is not expected to be significantly different from that for tip loading.

Eigenvalue Analysis

Karamba3d can also perform eigenvalue analysis.

In addition to the modeling of stiffness found in the static analysis so far, eigenvalue analysis was also performed to confirm the modeling of mass as well.

Calculation of predicted values

Each predicted value is calculated by the following equation. The values with subscript \(b\) are the natural frequencies for bending, and those with subscript \(t\) are the natural frequencies for torsion.
The torsion constant \(J\) is an approximation of the following equation, since the object is a rectangular cross section.

\(n_{b1} = \frac{1.875^2}{2\pi L^2}\sqrt{\frac{gEI}{\rho A}}, \\
n_{b2} = \frac{4.694^2}{2\pi L^2}\sqrt{\frac{gEI}{\rho A}}, \\
n_{b3} = \frac{7.855^2}{2\pi L^2}\sqrt{\frac{gEI}{\rho A}}, \\
n_{t1} = \frac{\pi}{2L}\sqrt{\frac{gGJ}{\rho I_p}}, J = \frac{0.422}{3}a^4\)

Boundary conditions

The boundary conditions are fixed at the base end as in the previous analyses.

Analysis time

The analysis time for eigenvalues is the time required to extract 10 modes.

Analysis Results

The results are shown below.

Results were compared for a total of five eigenvalues: in-plane bending, out-of-plane bending, first and second order modes of each, and first order mode of torsion.

Since it is difficult to see results other than torsion in the above graph, an enlarged version is shown below.

As can be seen from the eigenvalue analysis results, the Karamba3d shell element is torsionally stiff, as is the analysis under torsional loading, while for bending it is as accurate as an Ansys first-order element.

Conclusion

To get a more accurate result, it is necessary to check the values by changing the number of mesh divisions and measuring the analysis speed not once but multiple times.

We have found that Karamba3d is highly accurate for beam elements, not always close to the predicted values for shell elements, and very fast in terms of analysis speed.

In most cases where structural analysis is performed in Grasshopper, there is a need to run a large number of analysis models at high speed, such as parameter studies in the initial study.
Considering such a situation, the feature of being very fast with sufficient accuracy in the initial study is very much in line with the demand for structural analysis applications in Grasshopper.

We aim for better design not because the results do not exactly match the predicted values, but by using this knowledge to select the appropriate software for the level required for each design content and phase.

Appendix.

If you are interested in the Shell element of Karamba3d, please refer to the following paper, which can be found on the official Karamba3d website

• Tric: a simple but sophisticated 3-node triangular element based on 6 rigid.body and 12 straining modes for fast computational simulations of arbitrary isotropic and laminated composite shells.
  • J.H. Argyris, L. Tenek, and L. Olofsson.
  • Comput. Methods Appl. Mech. Engrg., 145:11–85, 1997
• The tric shell element: theoretical and numerical investigation.
  • J.H. Argyris, M. Papadrakakis, C. Apostolopoulou, and S. Koutsourelakis.
  • Comput. Methods Appl. Mech. Engrg., 182:217–245, 2000