by Javier Chavez, March 13, 2015

The Power of 2D (Axisymmetric Studies)

Back to Blog

In a world where 3D models are the norm, the days of 2D modeling are seen less and less. Sure, there are users that they only need 2D drawings and they still only use 2D tools even today, but for the most part, 3D is the most used type of modeling today. Simulation in general is no exception and it has come a long way to accurately calculate stresses, deformations, strains, reaction forces, and many other results in 3D models.

The other day I was working on a model in Autodesk Simulation Mechanical 2015 that was making use of axisymmetric study option. That is great because is made exclusively from 2D element types, and this simplifies the study tremendously as the nodes have only two degrees of freedom (Y translation and Z translation). Therefore, the time to solve is reduced drastically. Theoretically it makes sense because often we want to reduce our solving time using symmetry by cutting the part or assembly by half. The same could be done again and only analyze a quarter of it. Then we could do it again and only analyze an eight, and so on until we get a small enough slice to be represented as our asymmetrical cut section.


In fact, in Autodesk Simulation Mechanical 2015 you don’t even have to start with a 3D model and then slice it to a 2D. You simply start with a 2D element sketch and the software will know is perfectly axisymmetric as long as that option is used.

Now that we have 2D elements in mind, there are certain requirements that you need to fully understand when using axisymmetric studies.

2D elements must be input in the global Y-Z plane.

This is a simple to understand concept but could lead to potential issues if it’s not followed correctly. When designing the model to be used in the axisymmetric study, the “cut section” area of the part needs to be in the YZ plane. If your model does not lie in the YZ plane, you will need to modify it to ensure this orientation.

All elements must be located in the +Y half-plane where Y is the radius axis.

This is a complement of the first requirement where the positive Y plane needs to be used and it represents the radius of the axisymmetric part or assembly.

If a node lies along the axis of revolution (Z-axis) the translation in the Y-direction must be constrained.

This is assumption is often overlooked and could lead to incorrect results. Therefore it is always necessary to restrict the translational degrees of freedom in the Y-direction of all the nodes that lie along the Z-axis.

Nodal loads are normalized by the number of radians in a circle (load divided by radians).

This is perhaps the most overlooked assumption and can create confusion among most users. But it is important to know when reviewing the results. This basically states that the axisymmetric analysis only considers a 1 radian slice.

Figure below illustrates all the conventions previously mentioned.


Let’s take a quick example. Let’s image that we want to calculate the amount of force required to push a shaft through a rubber sleeve. The inner diameter of the rubber sleeve is slightly smaller than the outer diameter of the shaft.


First, I’ll start a ‘MES with Nonlinear Material Models’ study inside Autodesk Simulation Mechanical 2015 and I start modeling this two parts as 2D geometries.

Select ‘2-D’ as the Element Type.

Then I select ‘Axisymmetric’ as the Element Definition in 2-D. Notice  than when I select Axisymmetric the “thickness” changes to “1 rad”. This is to remind you that an axisymmetric analysis considers only a 1-radian slice.


Once the part is defined and I have assigned material, I could go ahead and generate the 2D mesh.

Then I proceed to setup the constrains. Since I modeled the axis of revolution to be coincident with the Z-axis, I need to restrain the translational degrees of freedom in the Y-direction. I also constrained the nodes in the shaft so they could only move in the negative Z-direction with a prescribe displacement to a certain distance to act as the push.

One important aspect to consider in this example is friction. Sure we could model this as a frictionless surface-to-surface contact, but if want to calculate realistic reaction forces we should consider a correct representation of the friction coefficients for the two materials that come in contact. In this example I simple used the ‘Modified Coulomb friction’ option with default friction coefficients.


Once I run it, I get my 2D results plot and I could animated it just as with any regular results plot.

One neat feature is that despite we only modeled this assembly as a 2D elements and we are presented with a 2D results plot, we could use the feature to visualize our results as 3D. To do so, I could simply right mouse click the part or parts I want to visualized and select ‘3-D Visualization’.

This is how our results look when the 3-D visualization option is enabled.

Once I have the 3-D Visualization, I could even add a slice plane to better visualize the von Mises stresses in the shaft.

Then, I could inquire the results of the nodes used in the prescribed displacement directly to calculate the sum of the reaction forces.

I could also graph those nodes to have a better visual representation of the analysis. As shown in the graph below, the static friction makes the reaction force increase upon contact and then the dynamic friction makes the reaction force increase gradually as more surface of the shaft comes in contact with the surface of the rubber.

Once I obtained the sum of the reaction forces, it is important to remember that since axisymmetric studies only consider 1 radian, I need to multiply my reaction forces by 2 π to obtain the required force to push the entire shaft.


All 2D approximations like plane stress criteria, plane strain criteria, axis symmetric criteria reduces 3D problems into 2D problem the main benefits of this 2D approximation is reducing the computing time, as number of elements are less the most accurate mesh can be generated and convergence error will be reduced therefore very accurate results will be obtained. But in case of 3D analysis too many elements too much of care required while meshing takes more computing time chances of errors will be more therefore whenever the problem meets the 2D approximation criteria it is best to go with 2D FE analysis

Back to Blog

Leave a Reply

Your email address will not be published. Required fields are marked *

More stories from KETIV


Quick Tip: Morph vs. Parallel Toolpath

HSM Quick Tip Video With surfacing toolpaths, the biggest struggle is figuring out which strategy will yield the best surface finish while at the same time giving you an efficient toolpath. In this quick tech tip we outline the difference between…

Read post

What's New in Inventor Nastran 2020

What’s new in Inventor Nastran 2020? The newest release of Autodesk’s flagship finite element analysis software, Inventor Nastran 2020, sees some major changes compared to previous versions. From an improved user interface to automated…

Read post