Showing results for 
Search instead for 
Did you mean: 

Topology Optimization: Result not as expected




A few weeks ago i wanted to simulate a contact between a plate and four rails:


Now i wanna do a topology optimization (TO) to reduce the volume of the plate but retain the stiffness (as much as possible...)


First of all: The TO needs the 101 solver i guess?! So i applied the loads (picture), fixed and symmetry constraints. Gravity force is not possible in a TO, right?




In the TO i choose "optimize all elements" except the surfaces with fixed constraints and the loads. The restrictions are: max displacement of two nodes and the volume with <0.4 


result looks like: 




The first question: why is the result with symmetric constraint different compared to the optimization with the full body?:




furthermore i expected the result more like a "supporting framework"!?


is the result ok, or are there any suggestions to get a structure like this:




thanks in advance


Re: Topology Optimization: Result not as expected


maybe anybody knows at least why i get different results when using the symmetry constraint?

Re: Topology Optimization: Result not as expected


I have another questtion regarding the topo opt.



How do I seperate the design area from the rest of the body?


If I split the body with planes:




the body is devided in the FEA too...





when using the "devide face" command to create the design space, the optimization is only removing material from the top




last try with optimizing "all elements" and freeze the other elements:





the elements under the frozen areas will be removed...




How to i optimize only the two volumes in the middle AND calculate the FEA as a united body?

Re: Topology Optimization: Result not as expected

Siemens Legend Siemens Legend
Siemens Legend

Hi spell,


concerning your symmetry question: When I understand it right, the difference is that you used a symmetric FE model (with a symmetric boundary condition) compared to a full FE model with a symmetry constraint in topology optimization. When I have it correctly in mind, the elements that are connected to nodes with a boundary condition are automatically frozen during topology optimization. That explains that elements in the symmetry plane remain in the resulting design for your first solution. I have to check if it is possible to toggle this behaviour in topology optimization.


If you would like to have a "framework" result, you could maybe check the maximum membersize parameter. Typically if you use a finer mesh, you would also get more bionic framework like structures. Maximum membersize filtering helps to keep smaller structures. The maximum memersize sholld not be smaller than 2-3 times your average element size.


Be careful during meshing your design domain. If you setup a mesh for topolgoy optimization, you should turn off the "Growth Ratio" in Tet meshing command in NX CAE to get a homogenious mesh size. (just turn the slider to 0.0).


If you want to control the frozen domains and you only select polygon faces to be frozen, only the elements connected to the face are frozen during the optimization.
If you want to freeze a complete block, I would recommend to use the SPLIT command and apply Mesh Mating Conditions. Mesh Mating Conditions are generating coincident meshes on the common surface - no glueing is needed. You can set the mesh Mating if you use the Split Command in Advanced Simulation on the Idealized Geometry. If you split in Modelling, you will not see the checkbox for automatic generation of the Mating Conditions. There is a customer default to see the simulation settings in Modelling - you can also generate the mating conditions manually in Advanced Simulation in the FEM file. Using Mating conditions you can run the Simulation on the complete body and define the design area on a subset. That should be exactly what you need.


Hope that helps you running your optimization successfully.


Best regards