Result without BCs

Hi Raphael,

I need a bit clarity on your query.

Is it a case like you got some results when no loads or BCs are applied to the model or a case like the solver runs even though we have not assigned any loads/BCs in the model?

Hi Georges, 

It's a mix of both. 

I've no BCs applied to the model, but I've a RWALL applied on it. No gravity.

A velocity is applied to the RWALL in order to impact the beam. The beam is not clamped, no BCs. I don't understand how RADIOSS is able to compute.

Thanks, 
Raphael 

explicit impact analysis doesn't require BCs

it computes behaviour based on time, as long as you want

Hi Tinh, 

I'm not sure to catch what you said. 

If I want to run this explicit impact analysis (see picure below), I've to block Z-translation of my beam, do you agree ? 

If I don't block any node, when the impactor will impact the beam, the beam will fall, right ?

<?xml version="1.0" encoding="UTF-8"?>

Hi Raphael,

Yes, normally the beam should fall. But what's happening in your case?

Can you please share the model file and h3d file.

Hi Georges, 

In my case, the beam is not falling ; it's like BCs had been applied to the beam.

Please find attached the model and results files.

Thanks for your help.

Raphael 

Unable to find an attachment - read this blog

Hi Raphael,

In you model the mass added is very high (115%) which makes the model to behave like this, as it is getting added to the structure.

Run the model without imposing any time step (remove /DT/NODA/CST) and we can see that it is behaving as intended.

<?xml version="1.0" encoding="UTF-8"?>

Yes, when the beam is too heavy in compare to impactor, it just moves a bit and seem to be fixed, you may have to plot displacement to confirm constraints, not only looking

Hi, 

Thanks for your support guys, it works perfectly ! /emoticons/default_smile.png' srcset='/emoticons/smile@2x.png 2x' title=':)' width='20' />

Raphael

Hi @George P Johnson, 

I placed some BCs on the beam in order to get the flexion and it works.

Nevertheless, I can't raise the velocity of the RWALL without having errors with mass.

I already compute the flexion with a 10 mm/s velocity, but now I want to change the velocity to 9150 mm/s. 

How can I do this without errors ? 

Thanks for your help, 

Raphael 

HI Raphael,

Are you getting an error like high mass error?.

If so, reduce the Tmin (target time step value) in /DT/NODA/CST keyword. Ensure the mass added (DM/M, which you can monitor in the engine out file) is less than 5% (.05).

If not, please share the engine out file.

Hi Georges, 

I reduce the Tmin as you mentioned, but I still have a DM/M=1.71 since the first step.

Then, I've got error code 207, RUN KILLED TOTAL MASS ERROR LIMIT REACHED

DM/M = 1.58e+259

Please find attached the .hm file concerned.

Raphael

Unable to find an attachment - read this blog

Hi Raphael,

In your model the rigid cylinder is having very high mass and velocity. This 'heavy' impact of the rigid cylinder on to the beam actually ruptures the beam elements which makes the time step to drop badly. And meantime mass will be added accordingly for maintaining the time step and finally the mass added reaches a very high value (in your case e259) which terminates the run.

Hi Georges, 

Thanks for your help. How can I fix the problem ? I really have to compute the model with this mass and velocity.

Hi Raphael,

Please select all the nodes (base nodes) of the beam and apply the boundary conditions.

Also you can recheck the material parameters, ie it should be able to withstand this high impact.

Hi Georges, 

Whaat do you mean by selecting all the nodes of the beam ? The impact is located on the midlle of the beam.

Hi Raphael,

Even though impacting at the middle the shock of the impact will pass throughout the component.

So you can try fixing all the base base nodes in all directions and try running.

Hi Georges, 

I've reached to deal with mass error so far. Now, I've a new error when I want to compute this high speed test. 

**ERROR : TIME STEP LESS OR EQUAL ZERO

I don't have any contact interface.

How can I deal with it ? Thanks for your help

Raphael 

Hi Raphael,

The time step in your model is dropping during the run and which finally results in run termination.

From the engine out files check what is causing this issue. It could be an element, or node or interface.

<?xml version="1.0" encoding="UTF-8"?>

For an element, check the related material.There must not be an error in the units system that this data is given in. check the element size also.

For a node, check the characteristics of connected elements. If the node is on the master side or the slave side of an interface, this interface must be verified.

For an interface, the gap of the interface must be verified if some failure happens on the master or the slave side of the interface. Also check the interface for any penetrations.

Hi George, 

I checked quality of elements and there are okay. Also, I just have only one component, so I don't have any penetration. 

I heard about AMS method, I'm running it but I don't know what's different compared to an non AMS model ?

It there an other way to run the model without using AMS ?

Please find attached the .hm file.

Best regards, 

Raphael 

Unable to find an attachment - read this blog

Hi Raphael,

Fix these two sides and run the analysis. But still I presume some time step drop will be there. 

Since the model gives high deformation (as the rigid wall has high mass) the time step will drop, else you have to try providing some failure parameters.

Regarding /AMS: Advanced Mass Scaling or AMS is a time step control method, where AMS allows setting the time step to a higher value than the usual elementary or nodal time step during the run. By using this keyword users can run the model quicker than the normal run time.

You can remove the /AMS keyword from the deck file and also from engine file you can remove /DT/AMS so that the model will take the default time step and will run.