Prestress Normal Modes tutorial+

[manu.marjanen]

Hi everyone! I’m running my first Prestress Normal Modes analysis in Autodesk Nastran for an impeller, and I’m a bit unsure if I’ve set it up correctly. The goal is to study the natural frequencies of the impeller under centrifugal load caused by rotation. I selected Prestress Normal Modes as the analysis type, defined the material, added the centrifugal load and constraints in Subcase 1, and in Subcase 2 I only added the constraints. The calculation runs without errors, but how can I be sure everything is correct? I haven’t found any clear tutorial showing the proper workflow. Does anyone have a tutorial video or a PDF guide that I could use to verify my setup?

[John_Holtz]

Hi @manu.marjanen 

You could change the load, run the analysis,  and confirm the frequency changes.

John

[manu.marjanen]

Hi everyone,
Could someone make a short video showing how to set up the constraints and loads for Prestress Normal Modes Subcase 1 and Subcase 2?

I need to make the part rotate around the Z-axis at a specific rotational speed (i.e., under centrifugal force) and then extract the natural frequencies. I haven’t found such a video online or in Autodesk tutorials

[John_Holtz]

Hi @manu.marjanen 

You wrote that you need to make the part rotate around the Z axis. That is probably not true. That would imply the shaft is free to rotate about the Z axis, and I am sure that your shaft and impeller are connected to a motor/engine through a coupling, gears, pulley/belt, or similar mechanical connection. 😉

In other words, the model should not be free to rotate about the Z because something prevents that. In fact, you do not need to rotate the model at all. You just need the load that simulates the effect that happens when the shaft/impeller rotates, and that is the Rotational Force load.

In your original post, you said you applied centrifugal loads and got results.

1. Did you run a linear stress analysis and confirm the results with the centrifugal load made sense? This would confirm you model is setup properly and has the correct load. (Maybe add a side load to confirm the simulated bearings are behaving the way you need them to.)
2. Did you change the value of the centrifugal load in the Normal Modes analysis and confirm that a faster RPM leads to a higher frequency?

It is probably easier for all the readers (including me) to look at your model and make suggestions than it is provide a sample. Besides, you want to know what's right and wrong in your model, not what's right in some random model. See What files to provide when the model is needed - Autodesk Community.

John

[manu.marjanen]

Hi everyone,
I have a segment of an impeller for which I need to calculate the natural frequency under centrifugal load.
However, I keep getting the fatal error T2116 and I have no idea why I can’t get it to work.

[John_Holtz]

What is a T2116 error?

The STEP file is not helpful. For problems with Nastran, we need your Inventor model that has the Nastran input. The STEP file is just the geometry, contains no input, and is not helpful.

By the way, you cannot use a symmetric model for a modal analysis. Some of the natural frequency results will not be symmetric. A symmetric model will not be able to calculate results that are not symmetric.

John

[manu.marjanen]

Hi,

I’m attaching a model where I’ve been trying to run a Prestress Normal Modes analysis.
The analysis works fine for the full impeller, but I keep running into problems when trying to run it on the impeller segment. I’ve been fighting with this for a while now. 😒

If running the analysis on the segment simply isn’t feasible, then I’d at least appreciate guidance on how to properly set up the Prestress Normal Modes connections for the complete impeller. At this point I’m getting quite frustrated because I haven’t been able to make it work on my own.

Any help would be greatly appreciated!

[John_Holtz]

Thanks for the model. I see you are trying to use Cyclic Symmetry. Here is what you should do:

1. Do not use a symmetric model for a modal analysis. The modal results do not have cyclic symmetry, so the results will be wrong (or at least missing all the modes that are not cyclic symmetric.)
2. Open the Inventor Nastran help.
3. Search for Cyclic Symmetry.
4. Set the "Refine By" option to Technical Support. (That is, ignore the Solutions In Forum and Product Documentation for the first search and concentrated on the Technical Support articles first.)
5. The first hit describes how to setup cyclic symmetry. Autodesk Inventor Nastran 2025 Help | Cyclic Symmetry in Inventor Nastran | Autodesk
6. Step 1 of the article says "The cut faces need to be straight planes that pass through the center of rotation". Your model violates that requirement, so the analysis will not run. (Two of the cut planes pass through the center of rotation; two of the cut planes do not pass through the center of rotation. Cyclic symmetry cannot be used for this geometry.)

Let us know if you have any questions.

John

[manu.marjanen]

Hi,

You are absolutely right — it’s not possible to perform a modal analysis correctly using a sector model of this impeller. Now that I’m running the analysis with the full impeller model, could you please take a quick look and tell me if these constraints and loads seem correct to you?

From what I can tell, the results look reasonable.

Please see the attached PDF for details.

Here is the setup:

• The load is applied only in Subcase 1.
• The same constraint is used in Subcase 1 and Subcase 2.
• The constraint is applied on the inner bore of the hub.

I also have one more question:
How meaningful is it to evaluate stresses using just a sector (segment) of the impeller? Is it possible that the results would be inaccurate due to the geometry not being fully cyclic-symmetric? Would it be safer to evaluate stresses using the entire impeller model as well?

Any insights or recommendations would be greatly appreciated.

Thanks!
Manu

[manu.marjanen]

 

[John_Holtz]

Hi Manu,

I have some questions/comments about your new question of "How meaningful is it to evalue stresses using a sector of the impeller".

1. What analysis type are you using? (To date, you have only mentioned Normal Modes analysis. Although it shows stresses, the stress value is meaningless. A modal analysis also shows displacements; those displacement values are also meaningless! A modal analysis only shows the mode shape. The mode shape is the same if you scale the displacements by any value X. The analysis "normalizes" the displacements to some value. Likewise, the stress results are some arbitrary value.)
2. Another way to think of it is as follows. In a regular Normal Modes analysis, there are no loads. Without loads, there can be no displacements and therefore no stress. Likewise, the Prestress Normal Modes analysis has "no load" for the natural frequency calculations. The loads applied in subcase 1 are just to change the stiffness of the model. The frequencies are calculated from the mass and stiffness.
3. To get real displacements and real stresses, you need to run some type of stress analysis. I believe you can make radial cuts so that you can use cyclic symmetry (even though that would cut through the middle of a blade -- that's not how you usually visualize the symmetry.) If that is true, the stress results will be just as accurate as analyzing the full model. I would make the cuts so that you have one full blade and two half blades. The cyclic symmetry constraints will be on each of the half blades. From the results, you will be able to compare the results at the symmetry faces with the full blade in the middle.

Of course, any type of symmetry requires the geometry, loads, constraints, and results to be symmetric. (Cyclic symmetric in your case.)

John

[manu.marjanen]

Hi, one more question! I attached an image showing the Loads and Constraints used in my Prestress Normal Modes analysis. Do these look correct to you?

[John_Holtz]

Hi Manu,

The model has a fully fixed constraint, has a load, and you like the results. I would say you did it correctly.

John