Nonlinear Static - Inertial Relief doesn't work with Free Constrain
Hi @Anonymous ,
According to the help Inertia Relief is supported in STATIC solutions (analysis). To me, this means that it also should work in a nonlinear static analysis, but it does not.
I keep on running into the E5000 error too.
Your model is symmetric. You could analyse a quarter of your model with constraints and without inertia relief.
Would that be helpful?
Accepted solution
On the cutting faces you could use a frictionless constraint.
It prevents the nodes to move in the normal direction of the face you select.
The third direction (in your case the Z-direction) can be constrained by selecting a vertex.
See attachment and take a look at the file "Test-assy-01-Nonlinear Static.iam".
Thank you, Roelof! That was really helpful 😃
Just one more question. On the picture below you can see that I run nonlinear static analysis with Separation contact type between surfaces. But I see that on the deformed representation the surfaces intersect each other. Why this happens? The nonlinear analysis have to take into account surfaces which have not been in the direct contact in the beginning. It should be the reaction force on such surfaces, they shouldn't intersect each other.
Accepted solution
Hello @Anonymous ,
That is because you have set the Deformation Scale not to actual, but to a certain percentage (10 by default).
Based on that setting (percentage) deformations are scaled based on the largest dimension of the model.
That is why it looks like the part have penetrated.
This behavior is perfectly explained in this article on the Autodesk website. Have a look.
Hi again, and thank you! Your tips really help.
Sorry for off-top, but since I try to copy your method, would you please comment why do I get following situation (picture↓)?
Seems like that in you case the whole vessel moves toward the constrained in axial direction point, but in my case the vessel moves from this point. Why it happens? I've used the same settings.
Hi,
In the article How to analyze a submerged pressure vessel I see no submerged vessel, but some shape ↓
I have concrete example – a submerged vessel. Would you please explain, how should I constrain this body, to simulate/imitate Inertial Relief for a nonlinear static analysis? Thank you!
Hi,
Yes, sorry that. I just change one detail in the assembly I've sent to you – I've make a hole, ang this problem back. Take a look ↓
I attached also updated assembly. I thing that we can play with this one.
Once again. I need a universal method which will allow me to perform nonlinear static analysis for any pressure vessels. Inertial Relief work good, but it's doesn't work under nonlinear static analysis. The article "How to analyze a submerged pressure vessel" shows an example with some body/shape, but I need a real example. At least me can not understand how can I constrain my real assembly in the manner which was described in this article. I like your method (I remember I've used approximately the same method – a quarter of the model + frictionless supports before, in Ansys), but it seems like that this method fails for models with some more complected geometry.
Than you.
Hi,
Please, read also my previous comment. Once again. So, we are speaking about is it possible to find a universal method which will allow me to perform nonlinear static analysis for any pressure vessels. Inertial Relief works good, but it's doesn't work under nonlinear static analysis. The article "How to analyze a submerged pressure vessel" shows an example with some body/shape, not a real pressure vessels. I understand, that with this article you've tried to cover all possible cases for any type of pressure vessels, but at least forme it was a bit difficult to understand how can I constrain my real assembly in the manner which was described in your article. If you refer to this article, so would you please to take my assembly (attached), and constrain it according method described in your article.
This updated assembly has a hole on the top part. It lead to the problem I got before, when the whole model move in the direction from the constrained vertex, which is lead to stress concentration at the constrained point, and just bad simulate the Inertial Relief function.
Another problem. Look at the pictures below. Displacement on the left side is 0.201mm, but on the right side is 0mm (because vertex in the center is constrained to make nonlinear static analysis able). But on the next picture, you can see the displacement behavior under Linear Static (Inertial Relief activated). We have displacements on both ends, and they are different. That why I ask you, please, take a real container, constrain it according your method, and perform analysis. Thank you.
Perhaps this image and the reference to SUBMARINES in the article will make it more understandable what the "2D shape is". (The article was created after talking to TWO customers who are designing personal underwater vehicles. Yes, the real designs are more complex, but I didn't think that my drawing was so different that it was unrecognizable. LOL.)
The problem with your model with the hole is the loads are wrong: the reaction force at the Z constraint (-2969 N) is much larger than 0. If you want correct results, you need to apply the correct load so that the reaction force is 0. In other words, the HOLE is missing a load equal to 60 MPa times the area of the hole (pi/4*(8 mm)^2). With the -2969 N load applied around the inside diameter of the hole (in the Z direction), the reaction force is -3.26 N, and the results look like this:
My SI is not very good, but doesn't 60 MPa pressure correspond to a water depth of approximately 6 km? In this case, the displacement of the model is 6 km + 0.201 mm, not 0.201 mm! What's my point? That displacement is RELATIVE to something. In the case of a model with no constraints, the displacement VALUE at a single point has no meaning because it can be measured relative to any point. In your nonlinear model, it is measured relative to the Z constraint. In the linear model, it is relative to who-knows-what. What IS important is the displacement from one end to the other. In other words, the stress and STRAIN are the same regardless of where the single node is constrained in the Z, and the end-to-end displacement is the same. The max and min Z displacement changes based on where the Z constraint is, but who cares?
Here is the summary of the universal solution method for any unconstrained model (not just submerged vessels) that has balanced loads applied (sum of forces in X, Y, Z =0, sum of moments about X, Y, Z =0):
- Choose any three points anywhere in the model, as long as they are not in a straight line. (Three points not in a straight line define a plane.)
- Add constraints so that the model cannot move as a rigid body, but is free to strain without creating stress due to the constraints. See Figure 3. In other words, the model cannot move freely in X but can elongate in the X. Same for Y and Z directions. Same for rotation about the X, Y, and Z axes.
- The displacements will be RELATIVE to the constraints, but the STRESS and STRAIN are correct for an "unconstrained" model. (The updated article may explain this better.)
That is the best I can do for a universal solution. You have the constraints for your specific model.
By the way: your linear analysis with the inertial relief is giving WRONG results because of the following:
- The applied load in the X direction on the model does not equal 0. Therefore, the inertial relief adds load in the X direction to all of the elements so that (sum of force in X) = 0. Therefore, the reaction force in the X direction at the symmetry plane will be close to zero, and the results are wrong. This is a WRONG use of the inertial relief.
- The applied load in the Y direction on the model does not equal 0. Therefore, the inertial relief adds load in the Y direction to all of the elements so that (sum of force in Y) = 0. Therefore, the reaction force in the Y direction at the symmetry plane will be close to zero, and that is a WRONG use of the inertial relief.
- If you were to model the full vessel in linear and use the inertial relief with no constraints, and apply the same loads that you applied in the model you attached to the forum (pressure load but missing the 2969 load at the hole), the results would still be wrong (but approximately correct). The reason that they are technically wrong is because inertial relief compensates for this missing load (at the hole) by adding it over the entire model. These loads are different than if you apply the equivalent pressure load to the hole, and therefore the results are different.
Let us know if you have any questions.