Tensile Test on Elastomer

[iteEZMMZ]

Hello,

I've been trying for some time to simulate a nonlinear elastomer stretching in Nastran like in this video.

https://www.youtube.com/watch?v=pn5sUlT9oFw (I took this video by random selection from YB) 

Right now I'm just trying to set up a nonlinear simulation like this stretch. But for later he would introduce Material which is elastomer.

Would anyone know how this could be simulated or maybe it can't be done at all?

I would be grateful for any answer and any help.

[John_Holtz]

Hi @iteEZMMZ . Welcome to the Inventor Nastran forum.

You have a model, and you have it setup for an analysis. If your only question is "can it be done", the answer is yes.

You may want to go through this tutorial since it has a few things in common:

• Nonlinear static analysis and how to enter the Nonlinear Setup.
• Using enforced motion to move the model a desired distance. (This is what the test machine does: move the part a specific distance.)

Otherwise, let us know if you have any other questions.

John

[iteEZMMZ]

Hello @John_Holtz,

thank you for your reply. I probably didn't convey my question well.

I am very sure that this can be simulated, I managed to simulate the action very easily on the linear simulation. (Just to see that I am simulating the machine.) While I did not succeed at all with the nonlinear hyperelastic Material.

I tried different ways with enforced motion and different combinations. But I just couldn't make it. I took a regular rubber from the Inventor media library as an example.

So I was hoping that someone could get me some help or instructions here, because I didn't succeed in anything with the tutorials you mentioned.

Best regards

[John_Holtz]

Hi @iteEZMMZ 

We need a lot more details than "it did not work". For example,

• You did a linear analysis that worked. Did you do the linear analysis in Inventor Nastran or Inventor Stress Analysis?
• You said the nonlinear with hyperelastic material did not succeed. What were the material properties that you entered? Where did the properties come from? (Hyperelastic is a selection on the material dialog that has specific input. None of the materials in the libraries have the hyperelastic constants or stress-strain data needed for an analysis using a hyperelastic material model.)
• You selected a rubber from the library. One rubber material in the library is wrong for simulation (the one with a Poisson's Ratio of 0.5; somewhere in the math that leads to a division by 0), and the other ones are difficult to converge (the ones with a Poisson's Ratio of 0.49). Which one did you use? Try changing the Poisson's Ratio to 0.48 if using the rubber as an isotropic material model.
• What did not work in the nonlinear analysis? Was there an error message? Did it not make it as far as the first output step? How many increments did you use? Did you set the Intermediate Output to "On" or "All" (as was done in the tutorial)? Did it run but the part did not stretch? Does the face with the enforced motion also have a constraint applied (as was done in the tutorial)? In other words, an enforced motion needs a constraint applied at the same location and in the same direction. The enforced motion moves the constraint; the constraint moves the model.
• When you say you did not succeed with the tutorial, what does that mean? Did the analysis fail to run? Was the tutorial not clear about what it was doing? Something else? (Some version of the tutorial did have some mistakes in the contact setup. I do not remember which version was corrected. What version of the tutorial did you use?)

In the future, please provide the current model that has the setup you tried. That way, we can see what you did and help with what needs to be done different.

Otherwise, I revised the original model you provided. The original had a force load and Generic material properties (which are correct for no material that I know of). See the attached file. These are the changes I made:

1. Added a rigid connector to the pull end. (This makes it easier to get the force required to pull the part because the reaction is at one node. See the image below. If you apply the enforced motion to the end face, you need to sum the reaction force from all the nodes. Inventor cannot do that AND graph the results.)
2. Used "Rubber - Butyl" from the library but changed the Poisson's ratio from 0.49 to 0.48 to make the analysis a little easier to converge.
3. Entered 10 steps and Intermediate Output "On" in Nonlinear Setup.
4. Added an enforced motion to pull the part 8 mm in Y.
5. Added a constraint to the same node as the enforced motion and fixed the Y direction. (You could also fix X and Z, too.)

Reaction Force to pull 8 mm (8 mm = Load Scale Factor of 1.0).

Note that I used Inventor Nastran 2023.

Let us know what questions you have.

John

[iteEZMMZ]

Hi @John_Holtz,

in order to perhaps better understand the changes and the way the simulation is processed, I would first ask one or two more questions before I jump back into this and solving the problem.

I wanted to open your model to see the settings you specified, but when I open the file it doesn't show the settings from the simulation.

Could it be that I am currently using Nastran 2022 and your model is from 2023?

Or is there another way to open the simulations so that I can see them too?

Let me try to answer the questions you asked me.

-I used linear analysis in Inventor Stress Analysis, just to see if I could simulate the movement like in the video. It was very simple even in many ways. Whether I put one end stationary and pulled from the other or pulled from both sides, it worked.

-That Hyperelasticity is currently causing me a problem, I'm looking for exactly the input I need for the simulation to succeed. Would this input be of help to me because of the material? Engineering Strain & Engineering Stress?

-What you state about the hyperelastic material means that I cannot run such a simulation with any standard material from AutoDesk? I need a hyperelastic simulation for this type of material. If I remember correctly all the experiments, I had no problem if I set some x Material, isotropic and to perform the simulation. The only thing is, I didn't succeed with a forced movement, only with force. But the results that were obtained simply did not make sense.

-As for Error, as I tried in different ways, I had several different problems. E5008, E5073, E5000, E5074, E5076, E5004 etc.. I tried with 5, 10, 20, 40 increments, as I wrote above, with forced movement I was not able to do a simulation at all, and my Output was always on all. Can you post a picture of how you verified the combination of constraint and forced displacement? Because I don't think I understood very well how to apply it.

-It was very difficult for me to find any tutorial with which I would be able to do this simulation, nonlinear and hyperelastic combination with these movements or moves like in the video.

So I had to research different tutorials and try to combine something.

So I would ask again, this file that you uploaded. Can I open it to look at your settings and how it was done?

And, I am currently using Nastran 2022.

Thank you so much for your effort on this topic !

Best regards

[John_Holtz]

Hi @iteEZMMZ 

Here are your questions (Q) and my replies (A):

Q: I wanted to open your model to see the settings you specified, but when I open the file it doesn't show the settings from the simulation. Could it be that I am currently using Nastran 2022 and your model is from 2023?

A: Yes. You cannot use an older version of Inventor to open a newer version. Always specify what version you are using! Someone using 2021 or older would not be able to look at your model and does not want to waste their time downloading and opening your file. Someone using 2023 or newer does not want to revise the model and send it back to you because of the same problem. 🙂

Q: (Refering to hyperelasticity) Would this input be of help to me because of the material? Engineering Strain & Engineering Stress?

A: The nonlinear force vs displacement curve measured in the video is a result of the hyperelastic material. You will not get this behavior using an isotropic material. See this article: How to enter hyperelastic (rubber) materials in Nastran | Inventor Nastran | Autodesk Knowledge Netw...

The measured force versus elongation (equivalent to stress versus strain) is not a straight line because the material is a hyperelastic. Using an isotropic material will result is a straight line (unless the cross-sectional area changes drastically).

Q:  I had several different problems. E5008, E5073, E5000, E5074, E5076, E5004 etc.

A: E5000 and E5004 indicates the model is numerically unstable. It is hard to know what causes that without having the model that produces those errors, but it usually occurs because the model is missing a constraint that prevents the model from moving freely in one of 6 directions (X, Y, Z translation, X, Y Z rotation).

E5074 and E5076 indicate the analysis is not converging. This occurs because the stiffness is changing faster than the analysis can calculate. The model you provided is using a Generic material with a modulus of elasticity of 0.0001. The displacement with a full load = F*L/A/E = approximately 100N*16mm/(4mm*2mm)/0.0001N/mm^2 = 2 kilometers. No wonder the analysis has a problem transitioning from 0 displacement to 2 km!

You mentioned using a rubber from the library. "Rubber - Butyl" has a modulus of 2 which would give an approximate displacement of 100 mm. Even that is super large for a specimen that is 16 mm long in the necked-down tensile region (50 mm long over all) .

I am not familiar with rubber material, but I know they come in many different hardnesses. Does this mean that one type of rubber, say Rubber - Butyl, can have different material properties? Personally, I would not use the Inventor library for a highly "specialized" material such as rubber because the library is source is unknown. 

I may have mentioned that the Poisson's ratio of 0.5 does not work mathematically. (Technically, 0.5 is a valid and accurate number.) This value needs to be approximated as 0.48 or lower when using an isotropic material.

A finer mesh and more steps can help minimize variations from element to element which can be difficult to converge.

Q: Combination of constraint and forced displacement? Because I don't think I understood very well how to apply it.

A: You need to apply a constraint to the same geometry as the enforced displacement. You want to pull in the Y direction, so the same location must have a constraint fixed in Ty. The enforced motion does not move the model. The enforced motion moves the constraints, and the constraint moves the model. This is why you need to apply both.

Q: It was very difficult for me to find any tutorial with which I would be able to do this simulation, nonlinear and hyperelastic combination with these movements or moves like in the video.

A: Yes, because the mathematics of hyperelastics is complicated, and therefore the material input is complicated. It is hard to find an easy-to-understand document that describes the material properties. But if you use a reasonable (isotropic) material and reasonable load, you should be able to at least run the analysis. Your model has these three specialties; the metal forming tutorial includes the first two. (I linked to the 2023 tutorial which has the corrected figures for the contact setup. The 2022 and older versions has the correct write-up for the Bottom Contacts but the figure shows the input incorrectly.)

1. nonlinear analysis
2. enforced motion
3. hyperelastic

Please update your model to try again, and attach the file with the complete setup if you are having problems.

John

[iteEZMMZ]

Hello @john.holtz,

Now understand the process of forced movement and Constraints.

I found this tutorial for setting up a rigid connector. But I didn't manage to apply it on this model. I put it on one needle and it's not right. I managed to pull, but the bottom was only attached to the corner and not to the entire surface. How should I fix the rigid connector for the entire surface? Or is it possible from the corner?

https://knowledge.autodesk.com/support/inventor/learn-explore/caas/screencast/Main/Details/968df65c-...

if I just place the 3D model, you probably won't be able to see the simulation?
Somewhere I saw a topic about setting up a Model with simulation, so as soon as I find it I will post it. Because this simulation that I have, does not look 100% like this video.

[John_Holtz]

Sorry, but that example is just a crazy model to demonstrate something (I'm not even sure what it is trying to demonstrate). No real model would be setup that way.

This is what you want to do for the rigid body connector in your model:

1. For the Dependent Entities, select the face on the end where you want to pull.
2. For the Independent Vertex/Point, select "Point At Center".
3. Click OK. That's it!

Then apply the enforced motion and constraint at the work point created at the center point by the rigid connector.

John

[iteEZMMZ]

Hello @John_Holtz,

My simulation failed. "FATAL ERROR E5000: Singularity detected at grid 55 component 1"

What can cause an error in this simple simulation? I posted the Model (Pack & Go) that I simulated, can you find the problem in it?

[John_Holtz]

Hi @iteEZMMZ 

Your analysis has no constraint in the X or Z directions, and it only has a constraint in the Y direction on one end. The simulation is statically unstable as indicated by the E5000 error. That is not allowed in a static analysis.

I think you want the enforced motion applied to the rigid connector on the opposite end of the bar. See the revised model attached.

John

[iteEZMMZ]

Hello @John_Holtz,

let me understand what we got now and how we got it.

We closed one end completely with Constraints. T and R by XYZ. On the other side, we placed a rigid connector with a central point and set a Constraint according to TY for it, where it will be pulled with the help of forced movement. I probably misunderstood that we place a Rigid Connector on one end and a Constraint on the other end according to TY where it should be pulled. I understood that we will set a Constraint by TY and drag that only that Constraint.

---

The enforced motion does not move the model. The enforced motion moves the constraints, and the constraint moves the model.

---

The diagram you posted above, TY spc Force vs Load Scale factor, is that diagram for stress strain, MPa / % ? The letter N on the left side of the TY spc Force annoys me. Should it be MPa or is it just displayed that way?
And this above Node 1405. Did you have to choose a special Node for that diagram or how can I get a diagram like from the clip?

[John_Holtz]

Yes, your understanding is correct.

• The constraint on the bottom end is where the test specimen is held by the machine.
• The rigid connector, constraint, and enforced motion on the top end is where the test specimen is pulled by the machine.  (You use a rigid connector so that you can pull on 1 node and get the total force by looking at the reaction force in 1 node. Reaction force is the same as "SPC". You could apply the enforced motion and constraint to the top face, but then you need to sum the reaction force from every node on the face and create the graph manually. You can right-click on "Constraints > SPC Summation" to get the total force, but you would need to write it down for each increment and create the graph manually.)

The "TY Spc Force vs Load Scale factor" image that I provided is a graph of the reaction force ("SPC" in Nastran terminology) in the enforced motion. Because it is a force, the units are in Newtons (N). The horizontal axis is the fraction of the load. My applied load is an enforced motion (of 8 mm). Therefore, the horizontal axis is the same as 0 to 8 mm of displacement at the top of the test specimen. My graph is identical (in concept, different material properties of course) to the graph in the video. 

If you want stress versus strain, then you should create an XY Plot of Stress versus load scale factor, copy that data to the clipboard and paste it into Excel, then create an XY Plot of Strain versus load scale factor and copy/paste that into Excel. Then you can create a graph of stress versus strain. Note that you need to turn on the output of strain results before running the analysis. ("Analysis > Edit > Output Controls > Strain").

John

[iteEZMMZ]

Hello @John_Holtz,

I tried first with the same diagram as you posted above. However, it seems different to me. Before I start setting up the diagram in excel, let me solve this problem. Maybe I have to do something different in the settings?

I installed the new Nastran 2023 now, so I took the first file you posted above.

And this new document now shows me an error in Nastran 2023 (Fatal Error E5076: Maximum number of bisections permitted reached), so I will investigate that as well.

[John_Holtz]

Hi @iteEZMMZ 

The new XY plot that you show looks like a problem with the graph. If your computer is set to use a comma for the decimal symbol (such as 3,14159 for pi instead of 3.14159), the XY Plot is wrong. You can also change the "Typ" (Type) from "Linie" (Line) to (Line+Symbol). My prediction is that most of the data points shown by the symbol will be on the vertical line at Load Scale Factor = 0, and only one data point will appear on the line that slopes up to the point (1, 3.5).

John

[iteEZMMZ]

Hello @John_Holtz,

yes, your prediction is correct, it shows the same thing again.

Would it be possible to change the settings in Nastran or via the settings in the computer or how did you mean it?

Best regards

[John_Holtz · Accepted solution]

Hi @iteEZMMZ 

You need to change the decimal symbol in Windows. See Incorrect graph of XY Plot result in Inventor Nastran | Inventor Nastran | Autodesk Knowledge Networ...

John

[iteEZMMZ]

Hi @John_Holtz,

great, I found how to change it. Now I will try to make a stress strain diagram and see what it looks like.

[iteEZMMZ]

Hello @john.holtz, we haven't heard from each other for a long time, I hope you are well?

After my last post, I didn't manage to do what I wanted, unfortunately at the same moment there were complications, so I had to stop the tests. I have now rejoined this thread. Unfortunately I was not able to make this diagram as you explained.

Could you please show me in more detail how to make this diagram?

---

If you want stress versus strain, then you should create an XY Plot of Stress versus load scale factor, copy that data to the clipboard and paste it into Excel, then create an XY Plot of Strain versus load scale factor and copy/paste that into Excel. Then you can create a graph of stress versus strain. Note that you need to turn on the output of strain results before running the analysis. ("Analysis > Edit > Output Controls > Strain").

To begin with, I would upload the last saved File, because I probably entered other parameters regarding the characteristics of the hyperelastic material, so now the result are no longer the same as then.

Best Regards

[John_Holtz]

Hi @iteEZMMZ 

Stress and strain results exist in elements. You need to select an element in the XY Plot instead of selecting a node. Therefore the steps are:

1. "XY Plot > New".
2. "Element".
3. Click an element you want to use in the graph.
4. "Result Data > Solid Y-Normal Strain" or whatever value you want to graph.
5. "Show XY Plot".
6. "Copy Data to Clipboard".
7. Open Excel. Paste the data into Excel to get the data points for strain versus load.
8. "OK" to close the graph in Nastran.
9. "Result Data > Solid Y-Normal Stress" or whatever value you want to graph.
10. "Show XY Plot".
11. "Copy Data to Clipboard".
12. Paste the data into Excel to get the data points for stress versus load.
13. Create a graph in Excel of stress versus strain.

John