Enforced Acceleration - Large Displacement

[tyler.patterson2]

I am running a transient analysis that stresses an assembly using enforced acceleration. I have constrained the bottom face of the assembly base in all six degrees of freedom, and applied enforced acceleration of 125g's on the same face...

When I view the results, the whole assembly has displaced an enormous amount. If I examine the displacement of two points on the assembly, I can see a difference in displacement - so there is relative displacement... But I would not have expected the whole assembly to displace since I have completely constrained the base.

Is the large displacement of the assembly the software's way of enforcing acceleration? This makes sense to me because I cannot imagine how an object would accelerate without being put into motion... And I am comfortable with this as long as I still see relative displacements throughout the assembly as well, because all I care about is the relative displacement and the stresses. 

[John_Holtz · Accepted solution]

Hi Tyler,

You are correct: the results are showing the total displacement due to the acceleration. This is nice on the one hand so that you can find out how far the part is moving. (If the displacement is different that what you expect, then there is a problem!) On the other hand, it is inconvenient if you want to see how the part is deforming; that is, you want to see the relative displacements (relative to the support).

Fortunately, there is an option that you can add to the analysis to get the relative displacement results instead of the absolute displacement results. The procedure is as follows:

1. If the analysis has not been performed, or if the input has been changed (mesh, material, load, etc.), right-click on the analysis branch of the browser and choose "Generate Nastran File". This updates the file that is used when you run the analysis.
2. Click the pull-down above the browser and change it from "Autodesk Nastran Model Tree" to "Autodesk Nastran File".
3. Locate the line "DISPLACEMENT(PLOT) = ALL".
4. Click the middle button to edit the line.
5. Click the checkbox "Free Format"
6. Change the text to "DISPLACEMENT(PLOT,,REL) = ALL"
7. Click "OK".
8. Click the toolbar button "Run Nastran File".

If you run the analysis through the interface (meaning the "Solve > Run" button on the ribbon), it will overwrite your manual changes.

See the page "DISPLACEMENT" for more information about that line in the Nastran file.

[tyler.patterson2]

John,

Thanks for the explanation. I now understand the difference between displacement due to enforced acceleration and relative displacement within the assembly. I will use the shortcut you mentioned to analyze my assembly. 

I have one follow-on question:

Is enforced acceleration a good way to model a shock pulse on the assembly?

In the real world the shock is acting on the base of the assembly, so my application point is appropriate... however, I am concerned because when the assembly is shock tested, it is hard mounted to the shock table and experiences sudden direction/velocity changes instead of massive displacements ... therefore when I apply enforced acceleration in Nastran In Cad, the large displacement is not representative.

Would I be better off applying a sudden change in velocity to the assembly in order to replicate the behaviour of a shock table? Or is there a way to apply enforced acceleration without creating that large displacement of the entire assembly?

Thank you,

Tyler.

[John_Holtz]

Hi Tyler,

Your approach (transient) is okay assuming that you enter how the acceleration changes over time. (Or displacement/velocity changes over time -- whatever input load is known.) In other words, your enforced motion needs to duplicate the motion of the shaker table, in which case the displacements will not be large (unless your shaker is moving a large distance ).

In other words, analyzing the model with a constant enforced acceleration whose magnitude is equal to the peak at some instant during a shake test will not give the same result in general.

[tyler.patterson2]

John,

I am providing a load scale vs time curve that dictates how the load varies over time. The error was in my dynamic setup inputs... I was applying the load for 1.0 sec when I meant to apply the load for 0.1 sec. 

My displacement is much more realistic now.

Regards,

Tyler.

[mark.solway2NMMC]

Hi John,

Is there a way to make the relative displacement change that you have described above a permanent change.

I'm having to keep changing this every time I run Random and Direct Transient response simulations as well as the TABRND1 row for the logX logY interpolation.

Regards

Mark

[John_Holtz]

Hi,

Inventor does not have the ability to make the relative displacements the default. You will need to edit the Nastran file and change the statements.

[mark.solway2NMMC]

Ok, thanks John