Learning Forum

[walsro]

I am in the process of simulating a body undergoing intense acceleration and deceleration. The body is an upside down U shape as seen below. It will be moving along a track, with wheels for stabilization. To simplify, the analysis conditions for a decelerating body will be listed: 

• initial velocity of 250 mph (-z)


• 1 g of deceleration (acceleration in +z)


• Deceleration lasts until velocity reaches 0 mph


• Displacement constraints applied at stabilizer wheel locations


• Approximate component loads applied (red faces)

 

So far, only non-converged results have been obtained. What might be keeping the analysis from converging? Is there a better way to setup the simulation?

Other than achieving converging results, the main goal is to ensure that the simulation is accurate to an actual deceleration on the track. Right now, dynamics and interactions between the pod components (motor, electronics, cooling, etc.) do not exist. What might be the best way of setting this up to account for moments, twisting, compression, etc., created by the components that will be mounted on the pod?

 
Should remote points be created and connected to the holes with each respective component weight applied at the remote point? Is it correct to apply an initial velocity, and then the deceleration (as we have done previously), or is there a better way to simulate a decelerating body? Any help would be appreciated.

[Sandeep Medikonda]

Hi,

What are the exact error messages observed in the transient structural simulation?
This might need to be debug based on the error being experienced one after another. 

Looking at the loads that the model is being subjected to. I am not surprised that the model is struggling to converge.
It is being subjected to almost 1/3rd the speed of sound. So, the inertial effects would be rather significant.
Have you considered modelling this Explicitly? Using Explicit Dynamics (AutoDYN) or WB LS-DYNA (not available in Academic) solvers.

It is recommended to use remote points to set up some of the load definitions due to better control over the rotational degrees of freedom and uniform transfer of loads. It is also recommended to use Joints and Joint loads whenever possible to simulate interactions. The use of point masses is another feature that the user has at their disposal in Explicit Dynamics.

It is recommended to simulate this as a multi-step analysis. 

For the application of initial velocity and deceleration. This will depend on how high the initial velocity values are? The inertial effects are changing direction depending on how high the initial velocity is, which might affect the contact forces etc. Based on the application of this model, it looks like this will be high in which case it I would recommend including the initial velocity and deceleration in different steps.

Regards,
Sandeep
Guidelines on the Student Community

[peteroznewman]

Hello walsro,

Please create a Workbench Project Archive .wbpz file to attach after you post your reply.  I will look at why it doesn't converge and advise on the correction needed.

A remote point can be created at the coordinates of the center of mass of each large object. The remote point is scoped to the holes that mount each object to the structure. A point mass is assigned to each remote point that represents the mass of the object.

Regards,
Peter

[walsro]

Peter,

Thank you for the response. The .wbpz file is now attached to the original post.

I have attempted remote forces as well as remote point masses (achieved higher simulation accuracy), neither of which has produced converged results. On my laptop, it has taken 6 hours to run the analysis for every attempt I have made. 

These are the messages that appear after the run has completed.

 

Thank you,

Rory

[peteroznewman]

Rory,

I ran the model attached (as is) on my computer. Here are a few observations:

(1) It only took 30 minutes on my computer, not 6 hours, but I allocated 12 cores and the solver allocated 13 GB of RAM to run the job. If your laptop has only 2 cores and 4 GB of RAM, that may explain it.

(2) The units were set to mm on this run. Not sure if that is what you used or if this was because those were the last units I had used on my computer, but that is not a good choice for solving. The reason is the magnitude of the displacement exceeds 1e6 during the solution and that is one of the ERROR messages. Run this model in m and the displacement will be 1e3 at this same point in the simulation. It got to 6.32 s. I reran the model in meters and it solved without any error.

(3) You said you wanted a 1 G deceleration, but the Acceleration BC shows -14.7 not -9.8 m/s^2 but more importantly, you need to apply 14.7 not -14.7 to slow down the initial velocity in Z.  The simulation is increasing the velocity, not decreasing.

Regards,
Peter

[srinivasagam89]

Thank you for the post. I have a situation where I need to analyze a model for 8g load condition. The main assembly gets connected to this model at mounting locations. Assembly weight is around 100 Kg. nCurrently I am running a static analysis with a input load of 8g*mass = 8000 N at the mounting location 2 mounting holes in Y-direction.nMy query is how do we simulate 8g condition? Do we need to run a transient analysis?n

[peteroznewman]

nMake sure all the mass in the assembly is represented in the model. Add a Point Mass if some mass is missing. You can see the mass in the model if you click on Geometry and look at the Details window.nUse a Static Structural analysis.nAdd an Acceleration load and type a value of 8*9.81 m/s^2n

[srinivasagam89]

Sorry for the late reply. Thank you so much. It worked and actually since it is a welding structure making them a single body gave better results and mesh connectivity.n