Inventor Nastran - Gravity (Load Type)

[jthomas2SNH8G]

I am trying to understand how the load type "Gravity" works in Inventor Nastran.

I've a simple FE Model of a 5"x2" Rectangular Cross-Section Plate that is 50" long.

One end of the block is constrained in all degrees of freedom.

On the free end I have a square block placed.

I run a linear static analysis with load type "gravity" to see how much the plate deflects.

I've run two cases-

1. Modified the mass of the square block to be 1000lb.

2. Modified the mass of the square block to be 2000lb.

Gave a=386.4 in/s2 and the appropriate direction.

Per my understanding - the gravity type analysis applies acceleration to all the notes and works in relation to F=ma where m is the mass of the component.

so, for the two runs I have I should be getting different deflections as I modified the mass. 

BUT that isn't what I see. I am getting the same deflection.

May I know what I'm missing?

[John_Holtz]

Hi @jthomas2SNH8G  Welcome to the Inventor Nastran forum.

My guess is the mass of the block did not update properly.

1. Does the support reaction match what you expect for either the 1000 lb block or the 2000 lb block? (Right-click on the constraint in the model tree and choose "SPC Summation".)
2. Did you change the mass density or the size of the block?
3. Did you remesh the model?
4. Is there a warning in your analysis and the displacement is really just for the beam and not the beam and block?

John

[jthomas2SNH8G]

John,

1. It doesn't match what I'd expect for a 1000lb load. SPC Force Summation comes to be 170.291lbf.
2. I changed the value of mass in the iproperties>Physical>Mass (General Properties)
3. Didn't remesh the model. Wanted to keep everything the same and just change the mass to verify that gravity was working how I was hoping it would.
4. The only warnings in my output are related to contact between the block and the beam (Bonded Contact). The max displacement value I'm reading is for the beam.

[John_Holtz · Accepted solution]

The reaction force sounds correct for the beam (or maybe the beam and block when everything has the density of steel).

The iproperties have nothing to do with the Nastran analysis. The mass in the Nastran analysis is based on the mass density (entered in the material properties) times the volume of the mesh. (The default is based on the material selected in Inventor, and that is also independent of the iproperties input.)

I think you found the problem. You need to change the material properties associated with the idealization that is used by the block. (The beam needs to be on a separate idealization so that "different" materials can be selected for the two parts: one part has material with real properties, the other part has material with adjusted density to give the desired weight.) A long time ago, you needed to remesh the model if the material properties were changed. I think that does not need to be done with recent versions of Nastran, but I am not 100% sure.)

John

[jthomas2SNH8G]

Yep, That solved it.

Thank you.