Remote Mass Loads

[Anonymous]

Is it possible to define a remote mass similar to a remote force? I need to run several dynamic scenarios on a trailer frame and I would like to define remote masses rather than modeling "dummy" cargo representing the actual mass and CG. Thanks!

I am running Simulation Mechanical 2013

[algor_neil]

Would nodal lumped mass do the job ?

[John_Holtz · Accepted solution]

Hi @Anonymous

To elaborate on algor_neil's answer, you need to create lines from the surface of the model to the location of the remote mass, and then apply a lumped mass at that location. There are many ways to do this. The easier methods are as follows:

• Use "Setup > Loads > Remote Loads & Constraints" to create the lines and add a lumped mass all within one command.
• Use "Draw > Design > Contact Elements" to create the lines. After that is completed, you can add a lumped mass.

[Anonymous]

Thank you both for the help!  I think I almost have it.  I do have an issue, though.  When applying a nodal weight (nodal mass is not an option) using the remote load dialog, the default "Mass/Weight" is set as "uniform".  I went with that since it was the default, which only gave me the option of inputting a weight in the X direction.  I thought that was odd, but went with it as the default.  The resultant vector was pointed in a random direction that I could not determine how it was calculated.  That seemed odd, so I unchecked the "uniform" option and defined the weight in the Y direction, which is the vertical direction in my model.  The resultant vector then appeared to be correct.  But, it doesn't seem to be linked to the direction of gravity.  This is important for my application because I will be considering the loading when the trailer is leaning due to uneven terrain or cornering.  My plan was to adjust the direction of gravity so it would automatically update all loads.

Is there a way to link the nodal weights to gravity, or will I need to adjust each one's specific directions for each load scenario?  Or, am I doing something wrong?

[John_Holtz · Accepted solution]

Hi @Anonymous

You should use the "uniform" option which indicates that the mass can vibrate in any direction: X, Y, and Z. (When the mass is equal in all directions, the arrow has components of [1, 1, 1] in the [X, Y, Z]. That is what you were describing as a "random direction".)

I have never seen a case where someone used  a non-uniform mass in all directions, but it is hypothetically possible. Think of a pulley that is attached to a shaft using a spline. If there is 0 friction between the pulley and shaft (and no pin or key to prevent sliding), then the pulley would be free to move axially. In this case, the pulley's mass would not affect the axial frequency of the shaft. But the pulley moves with the shaft in the lateral directions, so its mass does affect the lateral vibration of the shaft. In this scenario, you could represent the mass of the pulley using a nodal weight (nodal mass in the old days), and you would use a 0 mass in the axial direction and a real mass in the other two directions.

[Anonymous]

Thank you for the explanation.  I am getting closer to getting it to work.  After figuring out that I needed to change my beam material connecting the nodal masses to the frame to nearly 0 density, I am getting results closer to what I expect.  However, when running the simplest analysis (essentially duplicating a static analysis I ran with applied forces rather than masses w/gravity), I am getting a result with stresses approximately half of what I expect and displacements approximately 3/4 of what I expect.  The analysis I am comparing to was a simple static analysis with applied forces equal to the weight of the components.  It's results are in agreement with a basic Inventor FEA as well as hand calculation approximations.  All three indicate a maximum stress of 15-17ksi, so I am confident in that result.  The new model using masses results in a maximum stress of around 8.5ksi.  I wanted to validate the mass model before moving to different loading scenarios, which is why I am comparing.  I haven't had time to work with it today.  Is there anything you can think of that I should check before running another lengthy analysis?

Thanks!

[AstroJohnPE · Accepted solution]

Hi @Anonymous

I suggest that you hide the beam parts, exaggerate the displaced shape, and compare the displacement magnitudes of the two models (the static analysis with the force load to the one with the mass). Are the displacements being affected by the stiffness of the beam elements? If so, that might be affecting the stress results, too.

[Anonymous]

Thanks for the suggestion!  That worked!  I had selected surfaces rather than nodes when setting up the remote load.  So, I had dozens of beams going to each mass load, effectively adding substantial structure to the trailer frame.  I changed it to four trusses per load and now I am seeing more realistic results!  Thanks!