MES impact calibration

[Anonymous]

Hi Gents,

Trying to calibrate impact of the pendulum system in MES analysis type.

Please see figure below.

What am I doing wrong, after hitting solution button converging is taking hours, cannot see an end, while cannot reach second time step.

I have tried various parameters for analysis.

Would you have some ideas?

[marwan_azzam]

Hello,

Can you share the archive file with us?

[John_Holtz]

Hi there,

I just have questions. Perhaps they will help, perhaps they will not

1. Why are you using a beam element for the "rope"? A truss element should work better since the solver does not need to track the orientation of the cross-section.
2. Why do you have a spider of beam elements connecting the wire to the bricks?
3. Are those local coordinate systems on the bricks? What are they for?
4. If you delete the impact plane, does the analysis run?

[Anonymous]

Here it goes.

[Anonymous]

Thanks:

1. Wanted to make no hinge between end of the rope and brick sphere.

2. They are simulating fixed connection with center of the sphere.

3. To secure that impact plane will recognize 'correct' normals during the contact.

4. It does not help.

[John_Holtz]

Hi,

There appears to be something with the local coordinate system. When I remove them, the model runs.

I also changed the beam elements to truss elements. That makes the analysis easier to converge. (I was able to change the time step size from 0.01 seconds to 0.05 seconds.) Although it is acceptable to have hinge connections in MES, if you wanted to minimize the hinge effect, you could attach the rope to the top of the sphere (instead of at the center) so that the weight of the ball will reduce spinning about the X direction. You can use boundary conditions in the Tx direction to prevent the ball from spinning about the Z direction.

[Anonymous]

Thanks John, I am trying the same, however it is still ongoing.

My version of Simulation is 2015.01.00.0013, should I download any hotfixes or patches?

[Anonymous]

@John_Holtz I waited a little bit longer and it worked, thanks.

To reach the conclusion I would have now to extract the force which is generated in time of impact, could you help with this? I am inquiring some results in particular time step, but would like to get some advise.

[John_Holtz]

Hi,

I am guessing that the "Results Contours > Other Results > Reactions" are 0 between the wall and the ball. You probably need to activate the option to output the results of all time steps ("Setup > Model Setup > Parameters > Output" and check the box "Output results of all time steps".)

During the impact, the analysis will reduce the time step in order to converge, so essentially the maximum impact will occur "in between time steps". (The time step reduction can be seen from DT (third column in the log) decreasing and the L (fourth column) increasing.) If you are lucky to get any reaction forces during the impact, it is hard to know if you got the instant of maximum force or just some time step before or after the maximum.

[Anonymous]

I have performed as advised by you, however there is still 0 for reactions ('other results') reported at contact zone.

For further review I am attaching figure with some values.

Do you have any other ideas how to readout impact force in an efficient way?

[John_Holtz]

Well, that is unexpected. It appears that the option to output the reaction force at impact planes is not working. I am checking to see if there is a work around.

(One work around is to create one brick element to use as the impact plane, and define surface contact between the ball and "impact plane". This is what the software does internally when you use an impact plane. The summary file .AL shows what contact parameters were used during the analysis.)

[Anonymous]

I would appreciate if you could check what is wrong with reactions readout.

[Anonymous]

I have tried with your workaround and used one brick element together with surface contact definition.

Some error pop up, please see below.

What is advised to read out the impact force, please let me know?

[John_Holtz]

I suspect the "Program Exception" error was a random issue since the pendulum does not impact the wall until around 1 second. That is, the crash did not occur because something was occurring with the contact. But I do see an article at http://knowledge.autodesk.com/article/Error-forrtl-severe-157-Program-Exception-access-violation-in-... that indicates the problem could be caused by the number of contact elements. (One thing you might want to do is change the surface number of the lines on the ball where it impacts the wall so that you only have contact between a small area to the wall.)

If you run the analysis again, and if it stops at the same time step, then please attach an archive.

Regarding the reaction force with the impact plane, I tried to change the variables that I thought needed to be set, but I was not able to get the reaction force. I have reported this issue to the developers.

[Anonymous]

Here is archive. Please assist with the force readout...

[John_Holtz]

Hi,

I was looking at this throughout the day but ran out of time. For some reason, the analysis is reducing the time step much earlier (before 0.9 seconds) than the time of impact (around 1.1 seconnds), and that has me confused.

One problem in your setup is that the material does not have sufficient input to use the "von Mises with curve" material model. The software does a calculation using the properties in the library, but the "Elongation" value in the library is 0. So, bad material properties are why the analysis was reducing the time step at 0.65 seconds. (When viewing the material properties using units of N and mm, the strain for the last data point is 1.4447E-17 which is obviously wrong. When using display units of lbf and inches, the strain for the last point is a negative number!) If you expect the ball to yield at impact, then you need to correct the material properties. Naturally, if the ball is not going to yield, then you should set the material model (under the Element Definition) to isotropic.

Let's touch base again tomorrow.

[Anonymous]

Changed to isotropic, still the same issue.

[John_Holtz]

Hi,

When you wrote that it has the same issue, is that the error 157 or not producing reaction forces?

I am using Simulation Mechanical 2017, and it did not produce the error 157 when using your model as provided. Using a few tweaks to the model, it tries to get to 0.9 seconds and then reduces the time step. After running overnight, it had rebounded off of the wall. So I would suggest upgrading to version 2017 if possible.

I do not understand why the analysis is reducing the time step at 0.9 seconds. That is too early for impact. So I am hoping to make the model more efficient so that it takes less than 12-24 hours to run.

[John_Holtz · Accepted solution]

At least in the version that I am running (Simulation Mechanical 2017), the analysis reduces the time step to a very small value because the option to "Invode automatic timestep reduction method" for the surface contact is turned on (checked). When it is turned off, my test model ran quickly.

I think this is the path to that option in Sim Mech 2015: right-click on the contact pair in the browser, then "Settings > Advanced > Time-step" tab. Uncheck the box for "Invode automatic timestep reduction method".

Let us know how that runs.

[Anonymous]

It worked well, thanks!

Rest is the matter of proper callibration.