topic Re: Different simulation results in Nastran in CAD and Inventor stress analysis in Inventor Nastran Forum

Different simulation results in Nastran in CAD and Inventor stress analysis

Anonymous — Mon, 13 Jul 2020 09:18:18 GMT

Hello everybody,

I have a problem with the FEM simulation of a component.

A simple shaft is loaded with torque via toothing, supported with a fixed bearing (just behind the toothing) and a floating bearing (on the other side). As a "reaction", the rotation of the shaft (in the central area) around its longitudinal axis is blocked.
The (static) simulation of an absolutely identical simulation model with a simple Inventor FEM module gives much more realistic results than (also linearly static) with Nastran-in-CAD, regardless of mesh (fineness), storage and loading with forces / torques.
The location of the highest stress and the general deformation of the component are similar in all cases and look adequate.

Summarized quantitatively
inventor-fem linear elastic: 465 MPa and 0.185 mm displacement
nasrtran in cad linear elastic: by 6500 MPa and 1.148 mm displacement

even with non-linear static analysis, Nastran shoots to infinity

where could there be an error in the model / what could be the cause?

(W10, Autodesk Inventor Professional 2019, Nastran 2019, volume elements, parabolic element order, same material and loads)

Thanks in advance!

Re: Different simulation results in Nastran in CAD and Inventor stress analysis

Roelof.Feijen — Mon, 13 Jul 2020 13:31:03 GMT

Hello @Anonymous ,

I agree with you that in a linear static analysis you would expect to Inventor Stress Analysis or Nastran In-CAD to give the same results within certain limits. It hard to tell from the pictures what causes the difference. Can you share the model? What update of Nastran In-CAD 2019 are you using. (When you have the Nastran In-CAD active in Inventor click on the About in the Ribbon).

Re: Different simulation results in Nastran in CAD and Inventor stress analysis

Anonymous — Wed, 15 Jul 2020 14:46:14 GMT

Hi @Roelof.Feijen,

Thanks for the answer!

sorry for being late

Autodesk Nastran In-CAD Version: 2019.2.0.288

Autodesk Nastran 2019 Version: 13.2.0.168

here is the model:

https://1drv.ms/u/s!Ar6w4JjGxraHjRgzLRCiKVefm1Ho?e=pO3Bnw

the FEM analysis is in the 1410122_TBR_Richtrolle.iam file.

Re: Different simulation results in Nastran in CAD and Inventor stress analysis

Roelof.Feijen — Wed, 15 Jul 2020 16:56:21 GMT

Hello @Anonymous ,

The moment load applied in Inventor Stress analysis is a total moment load. It is automatically equally divided over the 14 faces.

In Nastran In-CAD the specified moment is applied to each face, so in this case you need to divide the moment load by 14. In this case this is possible because you have 14 faces with the same area size.

The way the moment is applied in both Inventor Stress Analysis and Nastran In-CAD seems to be wrong in my opinion. On each face a moment will act, but not from the center of the axis.

In Nastran In-CAD you have the possibility to apply a Rigid Body connector to the faces and create a workpoint in the center of the axis. You can applied the total moment load to the workpoint created by the Rigid Body connector.

This is something Inventor Stress Analysis is not capable of and seems to me a more realistic solution.

Re: Different simulation results in Nastran in CAD and Inventor stress analysis

Anonymous — Thu, 16 Jul 2020 12:21:06 GMT

Many thanks for the detailed answer, @Roelof.Feijen!

Then i will attempt with reduced torque, accordingly with the number of surfaces and report back with results

Many thanks for the help!

Re: Different simulation results in Nastran in CAD and Inventor stress analysis

Anonymous — Wed, 22 Jul 2020 15:26:45 GMT

@Roelof.Feijen wrote:
... The way the moment is applied in both Inventor Stress Analysis and Nastran In-CAD seems to be wrong in my opinion. On each face a moment will act, but not from the center of the axis. ...

That's only right for Nastran In-CAD. Nastan In-CAD gives each face a separate moment with different axis going through the center of each face.

Inventor Stress Analysis does not only distribute the given moment to all faces, but also uses an average axis. Because all 14 faces have the same size and are in a circular pattern (axially symmetrical), each face gets the same portion of the load and the average axis is the axis of the shaft. That's why Inventor Stress Analysis does exactely what @Anonymous wants to have.

I made a more simple shaft to show the behaviour of Inventor Stress Analysis and Nastran In-CAD in different cases. The attached model is created with release 2018 to be sure that @Anonymous can load it. Here are the displacement results with similar mesh sizes and similar color bars:

This one is similar to what @Anonymous did in Stress Analysis and brings the expected result.

This is what to do, to get similar results in Nastran In-CAD. The rigid connectors stiffen the faces though. So the behavior not the same.

This is what @Anonymous did in Nastran In-CAD but with correctely scaled loads.

This is the same done in Inventor Stress Analysis, you need six separate loads here. In contrast to a single load distributed to all faces, each faces get twisted around its own axis.

Because in linear analysis a moment is a tangetial force, this is similar to the first case. (10 Nm is 740,74 N with R 13,5 mm)

This is the same solution in Nastran In-CAD. So this solution is nearer to the original case in Inventor Stress Analysis than the solution with the rigid connector.

In reality the Solution will be in between. The driving collar will add sone stiffness, but not infinite stiffness like a rigid connector.

I guess the original solution from @Anonymous in Inventor Stress Analysis is a good solution for this task and the solution with the tangential forces is the best you can do in Nastran In-CAD using a single part analysis.

Re: Different simulation results in Nastran in CAD and Inventor stress analysis

Anonymous — Fri, 24 Jul 2020 15:19:54 GMT

Extra großen Dank für den Vergleich von Ergebnissen mit unterschiedlichen Lasten @Michael.Puschner , - ist sehr anschaulich!

Re: Different simulation results in Nastran in CAD and Inventor stress analysis

Anonymous — Fri, 24 Jul 2020 15:22:06 GMT

Thanks again for the answer, @Roelof.Feijen

now everything worked at me!