Jump to content
vishruthdilip

Remaining time increasing.

Recommended Posts

Hello guys,

 

I am running a simulation using RADIOSS.  The remaining time is increasing continously. How do i sort this out? I have posted images below for your reference. Any help would be appreciated.

Thank you,

Vishruth 

 

image.png.fe9706601be5ebb9dd57107e0be2c0a1.pngimage.png.4fa4dd38b1fb481ce0480e344eb859e1.png

Share this post


Link to post
Share on other sites

Hi vishruthdilip

 

This is because the time step is dropping in your model. In this case while reviewing the OUT file, the time step drop is due to interface ID-3 in your model.

Check and remove any penetration/intersection causing due to this interface ID-3.

Still if the error exists try imposing a reasonable time step and run the analysis.

 

Thanks

Share this post


Link to post
Share on other sites

Hello @Pranav Hari

 

This problem still seems to persist! I have removed all sort of intersections and penetrations. I have run the model checker, and there seems to be an error ( rigid body id is different from master id). But i have read, that this does not make any difference to the solver. 

The model used to run fine, when I gave an initial velocity to the component against a rigid wall. Now that i have kept the component fixed, and given an initial velocity to the rigid wall(cylinder) the probelm seems to have occured again. Could you please help me with this? 

 

Thank you, 

Vishruth 

Share this post


Link to post
Share on other sites
4 hours ago, vishruthdilip said:

Hello,

 

This problem still seems to persist! I have removed all sort of intersections and penetrations. I have run the model checker, and there seems to be an error ( rigid body id is different from master id). But i have read, that this does not make any difference to the solver. 

The model used to run fine, when I gave an initial velocity to the component against a rigid wall. Now that i have kept the component fixed, and given an initial velocity to the rigid wall(cylinder) the probelm seems to have occured again. Could you please help me with this? 

 

Thank you, 

Vishruth 

 

Hello @Ivan

 

I have just created a self contact( TYPE 7) for the component. Are the above parameters, applicable to this self contact? Is it necessary to define any other contact interface?Also i used the above parameters you mentioned for the self contact! It still has the same problem. Just to clarify, my model has just one component. 

Share this post


Link to post
Share on other sites

Those contact settings are recommended for crash analysis, but it can also be used in other applications. 

 

You can try increasing the Gapmin in your TYPE7 interface which will allow the contact to work sooner and prevent node from penetrating so far. 

 

Its also possible to use  /DT/INTER/DEL in the engine file, and where if this time step is lower than the value given in this option /DT/INTER/DEL, the slave node is suppressed from the interface. 

 

Check the FAQ from Radioss Help on Timestep in the attached document.

 

It is really difficult to give useful advice without seeing your model.

 

Time Step.pdf

Share this post


Link to post
Share on other sites

Hi,

 

there is a secure dropbox, however I will not be able to access it as I am not (yet) affiliated with Altair. If you are concerned to share publicly due to confidentiality reasons, maybe you can set up somewhat different model with similar problem.

 

Sometimes the physics of the problem involves large contact forces in which case timestep drop is unavoidable. Another reason for timestep drop is because Interface type 7 does not deal with edge to edge impact. When the mesh is fine enough, edge to edge penetration is often followed by a node to shell contact. The main problem with edge to edge impact is the locking situations. If there is a change of load after edge penetration, locking is unavoidable since a node to surface contact is detected. This usually leads to high penetration; therefore, the analysis comes to a standstill as time step is reduced. If locking occurs, the use of interface type 11 in this area is necessary to solve the problem.

 

timestep4.jpg

Share this post


Link to post
Share on other sites

Hello @Ivan,

 

I let the simulation run. The remaining time increased, and then dropped back to normal , and the simulation is complete. My understanding is that this happens , during impact when the time step drops. What are the recommended values for the various parameters , while defining self contact using contact type 7. However, I am getting a very large energy error. And also the deformation seems to be very large, could this mean edge-edge locking has occured? How do i check for edge-edge penetration?

 

Thank you,

Vishruth

Share this post


Link to post
Share on other sites

Hi,

 

the recommended values for type 7 contact are already posted above, only the Gapmin parameter is model dependent. 

 

Review the energy balance in Hypergraph by loading the runname_T01 file and plot total, kinetic, internal, hourglass and contact energies. Review timestep evolution throughout the simulation. Compare the plots and try to identify the issue. 

 

Please go through chapter 17 Checks During & After Analysis in already mentioned free Radioss ebook (attached below).

 

There is no specific procedure for checking edge-edge penetration- just carefully observe the animation in slow motion and look out for element edges crossing- it helps to display Shaded elements and mesh lines. It can be helpful to request contact vector output by eng/anim/vect flags CONT and PCONT to check in animation where and when high contact forces occur. If still unsure, set up type 11 line interface (or type 19, which is a combination of 7+11). 

Crash_Analysis_with_RADIOSS.pdf

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now

×