Nonlinear Static - Inertial Relief doesn't work with Free Constrain

[Anonymous]

Hi,

If I run Nonlinear Static analysis, and if I turn on Inertial Relief (AUTO) it doesn't work together with the Free Constrain. Any ideas what inputs can I try? Thank you.

[Anonymous]

Hi John,

Appreciate your extended answer. Thanks.

OK, now I see your yellow submarine 🙂

• "...the sum of the loads must equal 0, and the sum of moments must equal 0" – yes, it is an important notation. I haven't knew that the Inertial Relief add some forces to equal them.

"That displacement is RELATIVE to something..." – Yes, but I thought that the program show the displacement in the relation to vertex original position. I think that it will be probably better to run separate calculation for each part in the relation to for example joint surfaces.

"...universal solution method for any unconstrained model" – I try to apply this universal method as it describe by you, but I get following error: FATAL ERROR E5076 MAXIMUM NUMBER OF BISECTIONS PERMITTED REACH

I attached assembly. Would you please to check it and answer what I did wrong?

The symmetry method with the frictionless supports and one constrained in axial direction vertex work OK, but I still can't use your universal method.

[John_Holtz · Accepted solution]

The model is not statically stable, so a static analysis has no solution. Let's take a look at the constraints one-by-one:

•  Constraint 1. Txyz. Prevents translation in X, Y, and Z, but does not prevent any rotation. (Since it is a solid mesh, using a rotation constraint will not do anything, so it is okay that Rxyz are not checked.)

• Constraint 2: Tx. Prevents the model from rotating about Y, but does not prevent rotation about X or Z.
• Constraint 3: Tz. Does not do anything. Model can rotate about the X axis (passing through constraints 1 and 3). Model can rotate about the Z axis (passing through constraints 1 and 2). 

The constraints should be as follows:

• Constraint 1. Okay (Txyz)
• Constraint 2. Txy. Prevents model from rotating about X axis and Y axis. Model can rotate about the Z axis (passing through constraints 1 and 2).
• Constraint 3. Ty. Prevents model from rotating about the Z axis. Model is statically stable.

Another problem is that the loads do not simulate a submerged vessel. The pressure is missing from at least 2 faces.

Another way to figure out the constraints is as follows. Since the model is symmetric and you know that it is statically stable when using symmetry constraints, just use similar symmetry constraints on the full model!

• Nodes 1 and 4 are on the X and Y symmetry planes, so apply Txy constraint. (The rotation constraints do not do anything on a solid.)
• Nodes 2 and 5 are on the X symmetry plane, so apply Tx constraint.
• Nodes 3 and 6 are on the Y symmetry plane, so apply Ty constraint.
• The Tz constraint can be applied anywhere in the model, and described in the previous posts. The model will be statically stable about all 6 directions (X, Y, Z translation, X, Y, Z rotation).

[Anonymous]

Hi John,

That was a great explanation. Now I see what was the problem. Thank you very much!

Just a couple of theoretical questions:

• What will be the main different between symmetry method (one quarter calculation), and this free body method (T xyz, T xy, T y)? That the symmetry method can be applied for symmetrical models only? What method will be preferable (in your opinion) if we have a symmetrical about 2 plains model?

• What will be a correct way to use the Inertial Relief function then? To equal forces manually? Can you give an example when the Inertial Relief method will be absolutely recommended? 

Thank you again!

[John_Holtz]

Hi,

The symmetry model will be smaller, so it will run faster, display the results faster, and so on. Also, it is easier to see the inside of the model with a symmetry model than the full model. 😀

The symmetry model also has the advantage of creating a face through the thickness of the model where you can control the mesh size. In the full model, you have (almost) no control over the mesh size inside the volume. So maybe you use a mesh size of 10 mm which sets the mesh size on the surface, but the elements going between the inside and outside mesh can be any size that the mesh decides to use. 

A symmetry model can be used anytime these things are true:

1. The geometry is symmetric.
2. The loads and constraints are symmetric.
3. The results are symmetric. (This is the important one that is not always true. For example, vibration results are not necessarily symmetric even when the other two conditions are true. It is better to use the full model when analyzing vibration and mode shapes.)

I am sure there are cases where the inertial relief is helpful or necessary, but off hand I cannot think of any. It comes down to the question of do you want the software to balance the loads for you and apply some unknown loads, or do you want to create the balanced loads.