# How to correctly add gravity force in CalculiX?

Hi there,

I am using CaculiX to calculate the structure deformation long flexible tube under gravity force. However, I am a little confused about Newton gravity constant when I try to add the gravity force using the following card:

*PHYSICAL CONSTANTS, NEWTON GRAVITY=6.67E-11

Eall,NEWTON

According to online instrument of Newton gravity constant ( *PHYSICAL CONSTANTS (mit.edu)), it is set to 6.67E-11. However, my results show that this value is too small, as the deformation is much smaller than theoretical solution. I have also tried 9.81, but I got the following error:

ERROR: increment size smaller than minimum
** best solution and residuals are in the frd file
*

My question is what does Newton gravity constant stand for, and which value should I set to correctly create the gravity force? Does anyone have idea about it? Thank you very much in advance.

Yang

According to documentation, on page 423, you need to use the *DLOAD keyword, the set name, the type (in this case, “Grav”), the magnitude (if using mm the magnitude should be 9810mm/s²) and the direction of the gravity vector (x, y, z in global coordinates). Also, remember to include the density of the materials (again, if using mm the density must be in ton/mm³).

Using PrePoMax as preprocessor for a simple example the input file is as follows:

``````*DLOAD
Internal_Selection-1_Gravity-1, Grav, 9810, 0, -1, 0
``````

No need to specify the Newton gravity constant, it is used for simulating gravity relations between bodies such as planets.

The documentation also includes an example of the syntax for gravity load:

``````*DLOAD
Eall, GRAV, 9810, 0,0,-1
``````

`Eall` is an element set that can be defined along with the definition of finite elements and contains all the elements in a model:

`*ELEMENT, TYPE=…, ELSET=Eall`

As a side note, there can be multiple gravity loads (acting in different directions) in a model. Also, it doesn’t have to be gravitational acceleration. Any acceleration can be applied to the model this way (e.g. deceleration of a vehicle).

Thank you very much for your detailed explanation! So if using m, the magnitude should be 9.81m/s², the density is kg/m³, right?

Thank you very much for your reply! I had seen this example before, but I just a little confused about the magnitude. If using 9810, does it means that the unit of length should be mm, and the unit of density should be ton/mm³?

Yes, here are the consistent unit systems, from Abaqus documentation: Thank you very much for sharing! I had a try just now, and it works well! Thanks again!