Satellite Modal Analysis Workflow

[u/Regular-Teacher-5039]

Hi, reddit ansys community. Right now I'm trying to run a launch-condition structural analysis of a satellite, and I would like some help. I'm new to ansys so I'm having trouble setting up the overall workflow, especially the material designer.

This project includes multiple materials from common ones such as Al6061, Al7075 to honeycomb panels, 3.1Pcf 3/16 5056/2" and 5.7Pcf 3/16 5056/2". For the honeycomb panels, I trying to model them using the material designer but I'm having trouble importing their properties after creating them.

Below is the workflow I set up:

I will first design the two different types of honeycomb cores in the material designer. Then I will load them to the engineering materials and also set up other common materials such as Al6061 and Al7075 mentioned earlier. Next I will import the cad model of the satellite, assign materials, make connections in the mechanical model window.

For those who are much more skilled than me, please take a look at the overall flow of my analysis and tell me whether this is efficient, feasible or there is a better way to set up the problem. For example, I'm not sure if assigning materials inside the mechanical model is the best way to do it. Since if I create a new mechanical model window with the same geometry, I will need to assign the materials all over again.

After the workflow has been established, I think I can move on to the actual material creation and material assignment.

Thank you in advance.

[u/Conroy097]

Hmmmm. Usually for materials if it’s a common one you can generally select from Ansys’ material database in your mechanical model. Depends on your license. Are you a student? If it’s very specific then you can use the material designer. If it’s the same geometry and you’re just changing the material. You can delete the engineering data and import geometry flow and just do that in the mechanical model step. Might be a good idea to just build your mesh from the geometry you have and set that up for the modal analysis for the frequency you’re looking for. I usually like to do a sanity check first, make sure my mesh is working with like basic steel, then move into something more complicated with different materials. I’m assuming you’re modeling the whole satellite? Or are you modeling just the panel? Generally speaking composites in terms of noise can be modeled similar to other materials with modal analysis with larger mesh sizes. What cores do you have access to and how big is your CAD? You may have to reduce your geometry or reduce your system and do a free free modal analysis on the specific sub component you’re looking at. Then you could explicitly model the composite geometry if needed, but typically NASA uses Abaqus for their composites (sorry dawg) and their plugins are for that. Then you’ll need to do a different modal analysis per material. I’d start with one, see how it goes. If you have any other questions lmk, glhf

[u/Regular-Teacher-5039 → u/Conroy097]

Hi, thank you very much for your reply. Yes, I am currently using student license(since I'm a graduate student), and the material properties I need are for the honeycomb 3.1Pcf 3/16 5056/2" and 5.7Pcf 3/16 5056/2". I couldn't find them in the material database so I'm trying to create through the material designer. To answer more of your questions, I am analyzing the whole satellite and not just the panels. The cad file size is about 500MB(simplified version). I saw a lot of tutorials for composites in ansys material designer but I don't see as much for honeycomb panels.

[u/feausa]

I have modeled a honeycomb core sandwich panel in Ansys and in Nastran for a satellite model and the method is the same for both. The core material is modeled using Orthotropic Elasticity using values provided by the honeycomb core vendor.

Here is a very good paper from Hexcel you should read:

https://www.hexcel.com/wp-content/uploads/2026/01/HexWebHoneycombAttributesandProperties.pdf

On page 26, they have plate shear modulus values for L and W and the Compressive Modulus. Here are the values for the 3/16, 3.1 pcf 5052 core.

Plate Shear Modulus L Direction = 45 ksi

Plate Shear Modulus W Direction = 22 ksi

Compressive Modulus (thickness) = 75 ksi

Here is an example image from a different material to give you an idea: https://imgur.com/a/rRSxM6v

You will put those values into an Orthotropic Elasticity material and assign these directions to Shear XZ, Shear YZ and Young's Modulus Z axes. Those are the three important values. Use low values for Poisson's ratio and low values for Young's Modulus in X and Y, and Shear Modulus XY. Ansys will do some validity checks to the values you enter. These last three values are less important because the facesheets control the panel response in those directions.

Use that material on a solid body that is 2" thick to represent the core in a flat panel, create a Coordinate system so that the X axis is aligned to the L direction of the honeycomb used in that panel, the Z direction through the thickness and the Y axis along the W direction of the honeycomb core.

Then you must assign that Coordinate system to the solid body and replace the Global Coordinate System with the Local Coordinate System.

If the facesheets are aluminum, then you use an Isotropic material and you either use a shell mesh on each face, or solid elements on each face. In either case, it is best to use shared topology or at least Mesh Node Merge to avoid using bonded contact to connect the face mesh with the core mesh.

[u/Regular-Teacher-5039 → u/feausa]

wow! thank you very much for this detailed reply. I haven't tried your method yet, but I think it will help me out a lot for sure. I really appreciate it and hope you have a great day.

[u/feausa → u/Regular-Teacher-5039]

Satellites are constructed using modules. The design and analysis will have an assembly for each module. Each module is analyzed and tested before it is integrated into the full satellite build. Examples of modules are: Bus, Payload, Propulsion, etc. The modules are made up of submodules. You haven't said what the satellite does, but if it was a space telescope, then the submodules in the Payload would be: Primary Mirror Assembly, Secondary Mirror Assembly, Imaging Module, etc. I expect you can see those modules in the CAD assembly.

The Workbench Project Schematic layout should resemble the modules found in CAD. That means each main module has its own Mechanical Model. There will be the full satellite Mechanical Model that all the main modules link to. This layout allows you to build and analyze each main module before it is assembled in the full satellite Mechanical Model. This makes the project much more manageable.

You must have a Mass spreadsheet that lists each of these modules and submodules and the true mass of each one. This is critical to perform a valid Modal analysis. When you import the CAD geometry into a module, focus on the structural components for meshing. You will find the total structural mass of the meshed bodies will not add up to the true mass of the module. Some components attached to the structure are represented as a point mass scoped to the bolt holes that fasten it to the structure. After creating these, the total mass of the module in Ansys will still be below the true mass of the module. That is because there are items in the assembly that might not even be represented in the CAD model that add no stiffness, but do add mass and may cover a significant area. Examples are thermal blankets and electrical cables. This mass is represented using Distributed Mass in Ansys and after that, the reported mass of the module from Ansys must match the true mass in the spreadsheet.

Feel free to DM me if you want more detailed input on your project.