Frequency response stress results higher than expected

[ChadSkaret7795]

I have an aluminum weldment with motor and fan mounted to incorporated base plate. Modal analysis results are OK using a concentrated mass to represent motor / fan, rigid links to base plate (4 holes).

For frequency response a constraint was added to concentrated mass vertex and enforced motion velocity of 7 mm/s placed there, matching fan alarm vibration level. Damping set to 2.5% critical. Deformed shape and high stress areas are in agreement with failures in the field, however stress levels seem extremely high - approaching 1,000 ksi.

Is there anything missing in the setup?

[John_Holtz]

Hi @ChadSkaret7795 . Welcome to the Nastran forum.

I do not know the allowable for aluminum, but I trust that 1,000 ksi is above the allowable (endurance limit, yield stress, ultimate strength, and everything else). The part will break which seems to agree with what is happening.

Without seeing the results and all the input, my guess is the high stress is either at or adjacent to a constraint, or at a stress concentration (such as a hole or sharp corner). Most likely the magnitude will go higher and higher when you use a finer mesh at that area. If this happens, it indicates that the mathematics cannot calculate the real stress. (This is a singularity, the inability of the math to calculate the real value.) You can ignore the result at the singularity and use surrounding values to determine if the material exceeds the allowable.

Regardless of the cause of the high stress (whether real or a singularity), you are performing a linear analysis. Linear means the calculation can go to infinity if you apply a large enough load. A linear analysis will indicate if the part will yield, but it will not give results of what happens after the model exceeds the limitations of linear.

John

[ChadSkaret7795]

Thanks John. I realize the singularity issue. I have reduced vibration levels on the analysis to match those of some units not showing failure. Stress levels still indicate failure (that is those areas near singularity) well above yield. As long as the setup sounds correct I will have to accept the results. I've already concluded the design is inadequate, the client is having a hard time accepting this as there is a large volume in the field.

[John_Holtz]

Hi @ChadSkaret7795 

I just had a thought while re-reading your original post. It sounds like the 7 mm/s harmonic load in the analysis is applied to the concentrated mass. My guess is the vibration sensor is monitoring the mass and that is why you applied the load there. (Maybe the mass is the vibration sensor?)

However, isn't the concentrated mass the "output" and not the "input" for the load? Usually the model is mounted on something that is vibrating (such as a vibration table to perform a sine sweep or a larger piece of equipment that is vibrating), and therefore the input load is through the constraints. In other words,

1. Add a "Connector > Rigid Body" to the locations that are currently constrained.
2. Move the current constraints to the center point of the rigid body connector.
3. Add the known load to the center point of the rigid body connector.
4. (There are two reason for using 1 rigid body instead of N constraints on n nodes, such as at N bolt holes. First, ease of getting the reaction force at one node instead of N locations. Second, one enforced motion is more efficient than N enforced motions (times n nodes on each N locations!).)

Here's another way to think about the problem. A load of X applied to the constraints causes a motion of the 7 mm/s at the concentrated mass. A load of 7 mm/s at the mass does not necessarily create a result of X at the constraints; this result could be lower or higher than reality. What you need to know (or find out) is what load X at the constraints cause a 7 mm/s result at the concentrated mass.

John

[ChadSkaret7795]

Hey John,

That makes complete sense - a measured response at the motor is a result of the complete system motion and reaction. Unfortunately the 7 mm/s is taken from data for the fan vibration level just prior to unbalance alarm - so it is in fact an input at the concentrated mass (file screenshot attached). Some of the measured vibrational outputs in the field are well above this value.

If I were to use your approach, what would be the "known load" - gravity loads or the typical enforced motion load?

[John_Holtz · Accepted solution]

Hi @ChadSkaret7795 

It sounds like you are doing the setup properly. The concentrated mass represents a motor/fan combination, and some type of imbalance causes the vibration that shakes the structure. Even if the 483 ksi stress is discounted as a singularity, I see stresses in the "green" range (~200 ksi) on the round corners of something (rectangular tube?) which do not appear to be a singularity.

The second part of your question, "how to do my method", is not needed for your analysis. But to answer the question for discussion sake, you generally use an enforced motion and set the subtype to acceleration (or velocity or displacement). Basically whatever the known load is. (BTW, here is a general article: Analyze a rotating component with an imbalance load | Inventor Nastran | Autodesk Knowledge Network. Since you know the velocity load, you do not need to use a force load to simulate the imbalanced mass.)

What may happen in reality is that the vibration is a transient event, not a sustained steady state event. In other words, something happens to cause the motor/fan to start vibrating. Before it reaches the steady state condition where the stress is calculated to be 400 to 1000 ksi, the stress gets high enough to cause failure. The frequency response is finding the quasi-steady state response of the system. Depending on the speeds, it might take several cycles to many seconds to transition from no vibration to the full steady state response. You could run a transient response analysis. The runtime could be long since you want 20 time steps per cycle and need to run the analysis for numerous cycles to see how the result builds over time.

Depending on what causes the vibration and how the vibration switches operate, perhaps many physical setups never run long enough with the transient vibration to cause damage. Perhaps the transient starts to build up but something else happens which causes the vibration to die down. (My new washing machine can really bounce when washing heavy towels. It has some type of sensor that either slows the spin cycle and/or injects water to try to redistribute the mass so that the vibration is acceptable.)

John