Surface contact sliding issue

[Anonymous]

Hello everybody,

I'm trying to simulate a traction test on a hook-shaped steel wire in order to measure its opening on Inventor Nastran 2021. 
A first axis maintain the hook in place by blocking itself in the bottom "round shape", while another identical axis is located through the top ring. My mouvement is such as the top axis will move up and the bottom one is fixed (see picture below). As you can see the final direction of the loading on the hook is made visible thanks to a sketched line. The true physics behind this loading is a sliding of the bottom axis from point 1 to point 2 as the hook is opening wide under the load (opening = the angle of the free end  in relation to the vertical widens).

I've already tried to go through separation, separation/no sliding and sliding/no separation types of contacts whitouth obtaining the required motion. In fact, I can see a little bit of sliding but the bottom axis looks like if it was stuck to the hook's surface.

Moreover, as it is somehow linked to a Hertz pressure contact situation I have read M. @John_Holtz  advices on the topic of the "Spur Gear Contact Simulation" but my tests didn't work for me.

Please find enclosed one of my test files.

Thank you in advance to all those who will help me!

Best regards,

Jean-François

[John_Holtz]

Hi Jean-François,

I think your model is not statically stable (because of the motion), so you should not use a static analysis. You should use either Explicit Dynamics or Explicit Quasi-Static or Nonlinear Transient Response.

I have not tested Sliding type contact in a large displacement analysis, but my guess is that it only works for small displacement analyses. You should use separation contact in this analysis. Be sure to enter the maximum activation distance for the contacts. You know what the analysis will do better than the software.

[Anonymous]

Hi John,

First of all thank you for your reply, I really appreciate.

As for your recommendation not to use a static analysis, I had already reached this conclusion and I'm glad to see that you have had the same idea.

For my case a transient response doesn't very fit to my problem that's why I've decided to go for an Explicit Quasi Static type of analysis.

Your guess on the field of applications for the sliding contact makes sense to me according to what I've seen in my testings sofar. So I'm going to try to focus more on the separation contacts as you suggest.

As for the creation of an explicit quasi static  analysis I have to admit that it is a first time for me, hence I'm not very aware of the various settings and their manipulation, despite some researches. You will find enclosed my test file for this analysis, my main issue is that after around 2 hours of computation I still haven't converged to a solution which seems a bit too long for me (even if there are contacts), do you have any opinion on that ?

Below are my contact settings, as you can see I can't modify the input value for the maximum activation distance and I don't know why (sorry for my software language in French).

As for the load I don't really know how to set this right to some kind of imitate a traction test so I've used the following parameters:

[Anonymous]

   

Again, thank you for tour time!

Jean-François

[John_Holtz]

Hi @Anonymous 

Before I forget,

• The explicit analysis does not require a "Maximum Activation Distance" for separation contact. I did not remember that. 
• Please change the contact stiffness to 0.2 for all contact types when using the explicit analysis. (A new analysis will default to 0.2. If an analysis is duplicated from nonlinear static or another "regular" Nastran analysis that uses a default value of 1, the stiffness does not automatically update.)

The explicit quasi-static analysis does nothing that you cannot do with a transient/dynamic analysis. In fact, the quasi-static analysis runs the explicit dynamics analysis multiple times. The duration is extended on each run to minimize the dynamic effects and approach a "static" analysis. So this is what I am trying:

1. Eliminate the upper and lower blocks ("Mors") since those have a lot of mass. Most of the force in a dynamic analysis goes into moving the upper block instead of stretching the hook.
2. Apply constraints and the load directly to the upper and lower shafts where they are in contact with the blocks. (I think the blocks are much stiffer than the hook and shafts, so the constraints simulate that the blocks are very rigid in comparison.)
3. I am trying an Explicit Dynamics analysis with a duration of 0.001 seconds. (The predicted runtime is approximately 10 minutes.)
4. I am using a half sine-wave for the "load curve" (the transient table data) for the 300 N force. This curve starts the load off slowly (so that it does not jerk the model), increases the load more rapidly in the middle, and slows down at the end to "ease into the final load".
5. Using a 2 mm mesh on everything. The time step required by the explicit analysis is related to the smallest element size. At least until you get the model to run, it is nice to try to reduce the runtime. (After it is running properly, you can add some mesh refinement to get a more accurate stress.)

Here is the load curve:

Here is the stress result:

If happy with this, the next step would be to increase the duration (and the load curve!) to further minimize the kinetic energy, and refine the mesh in the areas needed. (Both of these, the increased duration and finer mesh, will result in a longer runtime.) For some reason, I could not get the load to work in version 2021. I'm sure that you will avoid the mistake that I was making. 🙄 I ran my analysis in version 2022.

[Anonymous]

Hi @John_Holtz ,

Thank you for your very useful return. I've got a lot of questions for you but before that I've tried to run a new analysis that follows your advice and I've obtained close results from yours, which is nice. Now I can see the sliding movement that I expected. Even if the loading point is still not perfectly reached it is a huge progress!

You will find enclosed my model and the .FNO file which should be slighty different from yours and run with the version 2021 (explicit dynamic).

Here are my questions:

1) I suspect that changing the contact stiffness to 0.2 is linked to the difference between the shaft and the hooks materials, is it the case ? And is 0.2 a "general" value or something specific that needed to be determined?

2) By comparing your remark on the blocks  I assume that if I reduce the shafts in size (especially the top one) more of the applied force will go for stretching the hook as there will be less mass involved, is it correct ?

3) As for the kinetic energy values, am I supposed to aim near to a certain known value or is it subjected to my free interpretation? Indeed the final kinetic energy value that I've rached for my simulation is of 1.53e+03, but I don't know whether it is an acceptable value or not.

4) My main issue now is that I still don't quite understand how to choose effectively parameters such as the duration, the number of steps and how to create a good loading curve, based on these parameters. As I said before this type of analysis is a bit unusual to me, I will be glad if you could explain quickly me how you like to proceed in such situations. I assume that the changing of the loading curve will bring the bottom shaft closer to the final expected loading point.

5) I have also notice that the ring at the top of the hook isn't moving like the bottom of the hook did. Ven if it's secondary, it is supposed to change in angle a bit until it comes to the shaft, do you have any opinion on that behavior?

6) Finally, do you think I can use the loading curve to bring the force value back to 0 in order to consider the remnants of the deformations (in case of a plastic deformation)? Indeed the final state of the hook after its elastic return is of utmost importance for me.

I'm sorry to take your time with a lot of questions but I really thank you for sharing your knowledge and helping me!

Jean-François 

[John_Holtz]

Hi @Anonymous 

1. The contact stiffness of 0.2 in an explicit analysis is not related to the materials. It is not related to anything in the model. The value of 0.2 is what provides a stable solution in 99% to 100% of the analyses. (When we encounter that one analysis that does not solve with the value of 0.2, we will learn what it means to use different values. 🙂)
2. Yes, reducing the mass of the top shaft would result in more force going to stretching the hook. But reducing the mass density will cause the time step size to get smaller, so the analysis will run longer. Instead of reducing the mass, it would be better to make the duration longer, or to switch to the explicit quasi-static analysis.
3. Yes, the kinetic energy is what you want to reduce. The explicit quasi-static analysis does this by running an explicit analysis with a duration of T1. Based on the kinetic energy compared to the internal energy/external work, it extends the duration to T2 and runs the explicit analysis again. When the kinetic energy is a small fraction of the internal energy, it says that is the quasi-static solution. (The range is 1% to 2% kinetic energy.)
4. The number of steps in the explicit analysis does not change the results. You are specifying the number of output steps that you can look at. The results are the same if you look at 1 step (the last one) or have 20 steps and look at the last one. The time step that is used during the analysis is set by the solver based on the materials, mesh size, etc. (See Section 28: Explicit Dynamics Analysis and section 29 for some background information.) You can set the Duration and the load curve, both of which acting together determine how much kinetic energy is involved. A longer duration implies the load is applied more slowly, so that helps to minimize any vibrations. Using a half-sine wave for the load curve instead of a linear ramp also helps. (Another example is applying an enforced motion to indicate that the face moves X mm over T seconds. If you suddenly start moving a face on a part at X/T velocity, the rest of the part will often vibrate due to the instantaneous acceleration. So when using an enforced motion, you should also apply an initial velocity so that the part is moving at time 0, instead of needing to be accelerated.)
5. I will take a close look at this. I assume the entire hook rotates, but whether the top slides X1 mm while the bottom slides X2 mm, or the top does not slide at all while the bottom slides X3 mm, all depends on what happens to the shaft. (The bending of the shaft may help keep the top of the hook in the same position left-to-right.)
6. Yes, you can use the load curve to remove the load to see the permanent deformation. If running it as explicit quasi-static, you need to indicate ("Analysis > Edit") that there are 2 steps: one step for loading, one step for unloading. Then the load curve can be a simple ramp up and ramp down. The quasi-static analysis does the work of converting the linear ramp to the sine-wave to minimize the kinetic energy.

[Anonymous]

Hi @John_Holtz ,

A big thank you for all your very useful and clear answers! It's much easier to understand my model now.

As you told me I tried to use a different duration and loading curve and I've found slightly better results.

Here are my settings: 

  

However when I plot my different energy values, despite the fact that I find good results, the evolution of the curve is very different from the one in the training (below), do you think these "waves" are a problem ? 

  

Moreover the final loading point is still not quite reached after the sliding of the hook on the bottom shaft. I thought that it would be the case by increasing the duration but it's not apparently. I will have to look closer to thsi problem because it feels like the initial position of the shaft on the hook is the determining element and it's not a good thing for me (too unrealistic and unpredictible).

For information this model took me 2 hours 35 minutes to be solved with all my 8 processors used and the same 2 mm mesh than before, I don't know yet if I'm going to try to refine the mesh or not.

I will try to run a quasi static analysis again to see if the results are better.

Jean-François

[John_Holtz · Accepted solution]

Hi @Anonymous 

The graph looks good in regards to the energies: the kinetic energy is much smaller than the external work/internal energy. The graph does not look "ideal" in regards to the waviness. It looks like the hook is encountering some vibrations.

I am debating whether an enforced motion would be a more stable way to move the rod. The advantage is that the motion guarantees the velocity (of the top rod at least) is 0 at the end of the analysis if you use a sine curve. With a force, the model can continue to stretch due to inertia even though the force remains constant at the end. You would need to take a guess how far it needs to be moved to create the 300 N force. (You have a good idea from the current results and/or from the design.) From the reaction force in the enforced motion, you would be able to see if you reach or exceed the desired load of 300 N.

[Anonymous]

Hi @John_Holtz 

I've tried to run the exact same simulation but with an enforced motion instead of a force, indeed the graph looks very good and almost perfect according to the example that I have. Your guess was right!

Unfortunately for my study I can't use an enforced motion for various reasons and I'm forced to use a force value, but now I know where this "wave-like" shape comes from and I know too that it has little effects on my results. 

I'm sorry but I haven't had time to test anything else lately, I will try to in the upcoming days before coming back to you in case of any questions.

For information you have answered a lot of my questions and I think that after these last tests and hypothetical questions I will close the topic. Thanks again!

Jean-François

[Anonymous]

Hi @John_Holtz ,

After some last tests it appears that I have no more questions for you, hence I have accepted your last post as a solution. Thank you a lot for all your time and your perfect answers everytime! It deserves to be said that you are a very pleasant and competent professionnal.

Jean-François