topic Re: Nonlinear Static - Inertial Relief doesn't work with Free Constrain in Inventor Nastran Forum

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

Anonymous — Tue, 25 Feb 2020 08:37:39 GMT

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.

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

Roelof.Feijen — Tue, 25 Feb 2020 10:48:57 GMT

Hi @Anonymous ,

Can you share a little bit more of information? What message do you get? Can you share a screenshot or even better your model.

Did you only add a free constraint? What about forces? Reaction forces? Are you sure you have an accurate and realistic load balance?

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

Anonymous — Tue, 25 Feb 2020 14:29:49 GMT

Yes, sure. I attached two assemblies with different inputs: one for Linear Static, and another one for Nonlinear Static.

This is about Pressure Vessel stress calculations. Problem is that for me it is relevant to activate so-called Inertial Relief function, witch is allows me to run analysis without any constraints. More precisely, I use the Free Constrain for one of the vessel surfaces, and I use AUTO for the Inertial Relief. NASTRAN work perfect with these inputs. But if I try to run Nonlinear Static analysis with the same inputs, I get an error.

Here is the inputs.

Case 1, Linear Static:

Load type: Pressure

Constrain type: Free

Material: Any (I used titanium)

Mesh type: Parabolic, Project Midside Nodes checkbox is activated. Quality Midside Adjustment is ON.

Inertial relief: Auto

Contact type: Separation or Bonded

Max Activation Distance: Auto

With this inputs analysis performs without errors.

Case 2, Nonlinear Static:

Number of increment: 5

Load type: Pressure

Constrain type: Free

Material: Nonlinear, Elacto-Plastic, Tangent Modulus 1250, Yeild Criterion von Mises 895MPa.

Mesh type: Parabolic, Project Midside Nodes checkbox is activated. Quality Midside Adjustment is ON.

Inertial relief: Auto

Contact type: Separation or Bonded

Max Activation Distance: Auto

This type of analysis doesn't work with these inputs. Error type: E5000 SINGULARITY DETECTED AT GRID COMPONENT 3.

If I add any constraint to any surface (Constraint 2, type Fixed in the attached assembly), except the Free Constraint, then it will work. That's why I've write in my first message that is seems like that the Inertial Relief function with the Free Constraint simply doesn't work under Nonlinear Static analysis.

The task is to make able to run Nonlinear Static analysis with Inertial Relief function and the Free Constraint.

Thank you!

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

Roelof.Feijen — Tue, 25 Feb 2020 14:53:56 GMT

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?

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

John_Holtz — Tue, 25 Feb 2020 17:10:29 GMT

Hi @Anonymous

I agree with Roelof. The NASTRAN help implies that it should work with a nonlinear static analysis, but I noticed the following differences between the linear and nonlinear output files:

The linear analysis includes a number of springs from the inertial relief. The nonlinear analysis does not include any springs.
The linear analysis shows the parameter INERTIALRELIEF is ON. The nonlinear analysis shows the parameter is OFF.

From this, it appears that the inertial relief is not programmed to work with a nonlinear analysis.

I agree with Roelof's suggestion of using symmetry, and then constraining 1 node (pick a node, any node) in the Z direction. This will create a model that is statically stable. In cases where symmetry is not an option, then the suggestions in this article will help: How to analyze a submerged pressure vessel.

Note that this article needs to be updated. Based on recent work for another case, I have learned that these are requirements when the model has constraints, but the article does not mention these requirements:

If the model includes any constraints, the sum of the loads must equal 0, and the sum of moments must equal 0.

I will update the article in the next day or so.

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

Anonymous — Wed, 26 Feb 2020 13:07:42 GMT

Hi,

"You could analyse a quarter of your model with constraints and without inertia relief.

Would that be helpful?" – Probably. Can I ask you what type of constrain you have used? Some type og friction less support? Could you share you assembly? Thanks.

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

Roelof.Feijen — Wed, 26 Feb 2020 13:46:20 GMT

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".

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

Anonymous — Thu, 27 Feb 2020 08:47:57 GMT

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.

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

Roelof.Feijen — Thu, 27 Feb 2020 10:10:36 GMT

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.

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

Anonymous — Thu, 27 Feb 2020 12:57:17 GMT

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.

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

Roelof.Feijen — Thu, 27 Feb 2020 13:33:06 GMT

I guess that the force on the bottom (right side in the picture) is bigger than on the top. This causes the model to move to the left (+Z direction).

You applied a pressure load on the faces and changed your model. You created holes in the top part. The force applied to the faces=pressure/area. Because the area of the top is smaller now than the area on the bottom the assembly starts moving. I guess your displacement results are also higher than before. The loading is no longer symmetric, so applying symmetry to your model is now questionable.

I don't know your design intent, but one solution in this case could be applying a higher pressure load to the top or use force loads on the bottom and top.

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

Anonymous — Thu, 27 Feb 2020 14:25:38 GMT

I tried with bigger force from the top. It doesn't help. I just need to perform Nonlinear Static analysis to an unconstrained submerged vessel. If inertial release doesn't work in nonlinear static analysis, what can I do then?

You can probably help me to understand this method (take a look my next comment ↓). Thanks in advance.

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

Anonymous — Thu, 27 Feb 2020 14:21:15 GMT

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!

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

Roelof.Feijen — Thu, 27 Feb 2020 14:41:38 GMT

Please attach your model (assembly and part files) that contains the latest modification.

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

Anonymous — Thu, 27 Feb 2020 14:58:31 GMT

Sure. Here they are.

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

John_Holtz — Thu, 27 Feb 2020 17:17:52 GMT

Hi @Anonymous

The model that you attached is different than the model where you show the result of 1381.0 (is that a stress?), so this does not help. The model that you attached is setup properly, but I would make two changes:

The mesh needs to be much finer in order to obtain more accurate results.
You need to check the reaction force in the Z direction at the node that is constraint in Z. (Right-click on the Tz constraint, choose "SPC Summation", and set the subcase to INCR 3.) The model that you attached has a Z reaction of -48.9 N. My guess is the model with the 1381.0 result has a much, much larger reaction force in the Z direction.

A real submerged vessel would have a Z reaction of 0. (What type of "vessel" is only 95 mm long? I guess this is a jar or container and not a "vessel" like a ship. 😁) The nonzero result indicates that the pressure loads do not balance, and therefore the setup does not simulate a submerged vessel.

You could split some surfaces of the model so that you can apply pressure to equal and opposite surfaces of the same area. (This may not be the easier solution.)
The model with the 1381.0 result has holes in the top. Did you apply extra loads in the model to simulate the pressure that is acting "on the holes"? If not, that would explain why the Z reaction force is much, much too large.
Alternatively, you could delete the pressure from one of the existing faces (such as one of the chamfers) and apply a different pressure so that the Z reaction force is closer to 0.

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

Roelof.Feijen — Thu, 27 Feb 2020 17:23:42 GMT

I have got a strong feeling that you did not attached the correct files. This is what I see when I run the Analysis.

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

Anonymous — Fri, 28 Feb 2020 08:30:19 GMT

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.

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

Anonymous — Fri, 28 Feb 2020 10:17:14 GMT

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.

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

John_Holtz — Fri, 28 Feb 2020 22:10:18 GMT

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.)

Figure 1: A personal submarine for one.

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:

Figure 2: Correct results.

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.)

Figure 3: Constraints to simulate a free body.

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.