Modeling of springs as a boundary condition

[l_fromm]

Hello everyone,

I am currently trying to perform a calculation with Inventor Nastran 2020.

I have a solid model that is supported on six springs in reality. The springs each have a stiffness of 200 N/mm.

The springs sit in a holder (see picture). To model the springs, I connected the bottom surface of the holder to the center of the surface using a rigid body connector. I place the respective springs at this point. 

I entered a value of 200 N/mm for the stiffness of the springs in the longitudinal direction. I have defined the remaining stiffnesses as 0.1 N/mm, as I only want to look at the stroke oscillation of the system initially.

The first simulation I want to run is a modal analysis to determine the natural frequencies of the system.

This is where I noticed the first inconsistency in my simulation. When calculating the first five natural frequencies and associated modes, the system's stroke oscillation along the local Y-axis is missing. I calculated this natural frequency by hand. Since the stiffness of a spring is 200 N/mm, the total stiffness is 1200 N/mm in the Y direction. The mass of the solid is 790 kg. According to my manual calculation, this results in a natural frequency of ~ 6.2 Hz (in the Y direction).

I have also attached the results. This shows that the calculated frequency is not the result of the

simulation is available. Furthermore, the calculated natural frequencies of the simulation do not include a pure stroke oscillation in the Y direction.

In my opinion, the first three frequencies with ~ 0 Hz are due to the low transverse stiffnesses, as there is hardly any resistance to movement in the X and Z directions.

Now my specific question would be whether I have modeled the springs correctly as a boundary condition?
And why the natural frequency I calculated does not appear in the Inventor Nastran solution?
Even when refining the mesh, the solution values do not converge towards the natural frequency of 6.2 Hz.

@John_Holtz can you help me with this problem?

Thank you for your answers.

Best regards
Luca

[John_Holtz]

Hi @l_fromm 

Not sure what the analysis model looks like, but based on your description there should be 5 rigid body modes in X and Z translation and X, Y, Z rotation. Mode 6 should be the oscillation in the Y direction.

There must be some problem with the input since the calculated frequency is not the expected value.

• You can confirm the mass is correct from the output file (.out). Search for "CENTER OF MASS" or "P A R T   D E F I N I T I O N", both of which list the total mass.
• The spring stiffness can be confirmed from the output file by searching "B U S H   E L E M E N T   S T I F F N E S S   C O M P O N E N T   P R O P E R T Y   D E F I N I T I O N"

(The spacing in PART DEFINITION and BUSH ELEMENT STIFFNESS" may not be proper in the forum post. May be easier to scroll through the output to find them since Nastran writes out those titles with extra spaces between each character.)

John

[l_fromm]

Hi John,

thanks for your quick response.

You can imagine my model as a rectangular sheet metal construction. The component sits on the six springs mentioned above, which are arranged in parallel and are therefore purely spring-mounted in the Y direction. The arrangement of the springs is axially symmetrical to the longitudinal axis of the cuboid. The six springs are arranged so that there are two on the rear side and one on the front side of the component.

As far as the simulation is concerned, the six springs are the only constraint of the component. Overall, I would like to specify the different stiffnesses for the springs and use these as resistance to the movement. I have already calculated the transverse stiffnesses of the springs.

If I now specify three stiffnesses in X, Y and Z, then the system should have at least three natural frequencies as pure stroke oscillation in these directions, right?

The mass and the spring stiffness are correct, I was able to read that in the .out file.

Do you think that the error is due to the fact that I have no dependency in my model? So only the six springs and no other bearing?

Best regards
Luca

[John_Holtz]

Hi Luca,

Have you tried calculating more than 5 frequencies? The accuracy could be related to the number of modes (with more modes producing more accurate results for the lower frequencies).

If it is not that, I would suggest changing the Nastran file to add the value for CTOL on the EIGRL card. CTOL is the in the third field on the second line. Try a value of 1.0E-7. (See Autodesk Inventor Nastran 2025 Help | EIGRL | Autodesk).

John

[l_fromm]

Hi John,

I have tried to calculate several natural frequencies. Even with the selection of 50 natural frequencies, the calculated value was not included.

I have changed the CTOL value setting to 1.0E-7. Unfortunately this did not improve the results either.

I have now started to perform a linear-static analysis with the model, as I am also interested in the existing stresses in the structure.

However, since the component is only supported on springs, these springs would be the only constraints of the model.
As soon as I start the simulation, it aborts and I get the message that I first have to define constraints in order to perform a linear-static analysis.

Which constraints should I define now? I don't want to make the model stiffer with the dependencies.

Best regards
Luca

[John_Holtz]

Hi Luca,

Perhaps with 6 springs at "random" locations, there is no frequency that is purely in the Y direction at 6.2 Hz. If the center of mass is offset from any of the springs, the natural frequency is a Y translation and X or Z rotation at some frequency other than 6.2 Hz. Otherwise, I do not have any new ideas about why the modal analysis is not calculating the expected result. You should provide your model if you want someone to look at it.

For the linear analysis, the solution depends on what the specific error or warning is and when it occurs. My guess is you need to follow the instructions in Tip 8 in the PDF document attached to my forum post Suggested Reading - Tips and Tricks on the Inventor Nastran forum so that you can tell the analysis to run even though there are no "constraints" define in the model. (That is, Inventor may not be smart enough to recognize a grounded spring as a valid constraint.)

John

[l_fromm]

Hi John,

maybe that's the case.

In any case, tip 8 worked and I was able to calculate the model using only springs as a dependency.

I created two subcases in my solution. One with springs as a constraint and one with a fixed constraint.
Now the simulation shows that the stresses are significantly higher for the subcase with springs as constraint (twice as high for all simulations, regardless of the meshing).
In your opinion, is this a realistic correlation?

Best regards
Luca