Gravity Load Results in Excessive Stress & Deflection

[lhessRXVRV]

Hello,

I am running a Linear Static analysis and have discovered that including Gravity (-386.08 in/s^2) results in excessive deflections (~1,000 inches) and infinite stress levels in the structure. 

There are many loads within the subcase. If I remove the Gravity load from the subcase, the results seem reasonable (I compared the deflections to those found using RISA Structural Design Software). The stress levels also make sense and agree to hand calculations.

Are there any settings/parameters that need adjusted to correct this issue when applying Gravity? (This is the first time I am applying Gravity using the 2024 version).

Running Autodesk Inventor Professional 2024. 

Thank you in advance.

Luke

[John_Holtz]

Hi Luke,

Maybe check the reaction forces for the model without gravity and the model with gravity. (Or run the analysis with gravity alone if it doesn't take too long.)  I think you will find that the weight of the model is too high. (You check the reaction forces by right-clicking on the constraint in the model tree and choosing Reactions, or SPC Summation if the readers of this message are using an older version of Inventor Nastran.)

You can also search the output file (.out) for the word "mass". One of the hits will list the mass of each idealization and the total mass.

• If the total mass is wrong, it is due to the wrong mass density in the material properties. Remember that mass density = weight density/gravity. Steel in the English units is around 0.00075 lbf*sec^2/in/in^3/
• If the density and mass is correct, is it possible the gravity value needs to be in different units? For example, 9.81 m/s^2 instead of 386 in/s^2?

John

[lhessRXVRV]

Hi John,

Thank you for quick reply. I ran a gravity-only subcase after your suggestion. My model weighs approximately 16,000 lbs., originally calculated by Inventor, and the RISA software weight-takeoff was very close to that number. 

I have two constraints and am seeing a reaction of 8.9e+8 lbs. and 2.7e+8 lbs. Something is not right for sure...

I have verified that the units (at least next to the input box) are in in/s^2 for the gravity load. I have also verified that the material density for steel under the "Midsurface" features within Nastran are set to 0.00073454 lbf s^2/in^4. 

I had a feeling that density was set to an incorrect value after thinking about your reply, but that does not seem to be the case either.

Thanks,
Luke

[John_Holtz]

Hi Luke,

I cannot think of a reason. Can you provide the model? If so, use the steps in this post, and attach the zip file to the forum. What files to provide when the model is needed - Autodesk Community

John

[lhessRXVRV]

Hi John,

I was able to figure out where my mistake was... I am working with a model which includes midsurfaces, solids, and line (beam) elements. 

The only purpose of the line elements is to transfer load from a node into the structure. I want to give the line elements very high rigidity (based on a modeling assumption). I therefore gave the line elements a diameter of 1000 inches. However, not realizing I left the density as 0.00073454 lbf*sec^2/in/^3, which at a diameter of 1000 inches causes an excessive load when gravity is applied. 

I manually changed the density to of the line elements to 0.0 lbf*sec^2/in/^3, but left the modulus of elasticity unchanged to provide the correct stiffness/rigidity. 

Thank you for the help! Very much appreciated...

Luke