Model Coal Sloshing in Tank due to Inertia Using SPH
Hi,
I am trying to simulate coal/grain being thrown around in a container due to an inertial force/acceleration/velocity. I have attached my files in this message. I am very new to RADIOSS and I am getting several errors. The model checker lists:
-RBODY on element
I am following the tutorial in the attached .pdf and created my rigid body and supports according to those instructions.
-Part/mat/prop incompatible
The coal/grain is modeled as SPH elements. I am using MAT LAW 10 to describe the coal. Checking the reference manual it seemed this was the best MATLAW to use, but I am unsure. If there is a better one please advise. Also, if possible, please advise how the card should be filled out.
-Incompatible kinematic conditions on nodes
I assume this is because I have done something wrong with my supports, as when I isolate , that's what it shows. I created an SPC again, according to the attached tutorial.
I realize that likely a lot of what I have done here may be nonsensical. I am on an academic server, so I do not have access to many of the necessary tutorial files, especially those to do with SPH, so if you are able to provide some sort of tutorial/guide to follow, it would be greatly appreciated.
Thanks in advance for the help.
When I run in RADIOSS:
************************************************************************
** **
** **
** RADIOSS STARTER 2017.2 **
** **
** Non-linear Finite Element Analysis Software **
** from Altair Engineering, Inc. **
** **
** **
** Windows 64 bits, Intel compiler **
** **
** **
** **
** Build tag: 0871760_123352017.2_1020_0048655_10 **
************************************************************************
** COPYRIGHT (C) 1986-2017 Altair Engineering, Inc. **
** All Rights Reserved. Copyright notice does not imply publication. **
** Contains trade secrets of Altair Engineering Inc. **
** Decompilation or disassembly of this software strictly prohibited. **
************************************************************************
.. BLOCK FREE FORMAT
.. STARTER RUNNING ON 1 THREAD
.. CONTROL VARIABLES
.. UNITS SYSTEM
.. MATERIALS
ERROR ID : 829
** ERROR IN DRUCKER-PRAGER MATERIAL LAW 10
DESCRIPTION :
-- MATERIAL ID : 2
-- MATERIAL TITLE : coal
TENSILE BULK MODULUS IS LOWER OR EQUAL TO 0.
.. NODES
.. PROPERTIES
.. 3D SHELL ELEMENTS
.. 3D TRIANGULAR SHELL ELEMENTS
.. SPH PARTICLES DEFINITION
.. SUBSETS
.. ELEMENT GROUPS
.. PART GROUPS
.. SURFACES
.. NODE GROUP
.. BOUNDARY CONDITIONS
.. INITIAL VELOCITIES
.. DOMAIN DECOMPOSITION
.. ELEMENT GROUPS
.. INTERFACES
.. INTERFACE BUFFER INITIALIZATION
.. RIGID BODIES
.. RETURNS TO DOMAIN DECOMPOSITION FOR OPTIMIZATION
.. DOMAIN DECOMPOSITION
.. ELEMENT GROUPS
.. INTERFACES
.. INTERFACE BUFFER INITIALIZATION
WARNING ID : 343
** WARNING : INITIAL PENETRATIONS IN INTERFACE
.. RIGID BODIES
.. ELEMENT BUFFER INITIALIZATION
WARNING ID : 312
** INCOMPATIBLE KINEMATIC CONDITIONS IN MODEL
DESCRIPTION :
6 INCOMPATIBLE KINEMATIC CONDITIONS IN MODEL
.. GEOMETRY PLOT FILE
.. ERROR ==> NO RESTART FILE
ERROR TERMINATION
------------------
1 ERROR(S)
22 WARNING(S)
PLEASE CHECK LISTING FILE FOR FURTHER DETAILS
==== End of solver screen output ====
==== Job completed ====
(Directory info here)
Job load: 1
Restart file SPH Trial_0000_0001.rst was not created.
Missing 'NORMAL TERMINATION' in output file SPH Trial_0000.out.
'ERROR TERMINATION' in output file SPH Trial_0000.out.
radioss:: Solver run finished after 22 seconds.
Answers
-
Hi,
I have made the following changes:
1. RBODY on element
master node of a rigid body should be independent (not connected to mesh). When creating rigids, make sure the primary node is set to calculate node. Pick this master node of rigid body for boundary condition 'Support'.
2. ** ERROR IN DRUCKER-PRAGER MATERIAL LAW 10 TENSILE BULK MODULUS IS LOWER OR EQUAL TO 0.
You have provided only density for this material, which is insufficient to run. Please search the literature for material properties of coal. All material laws in the Concrete and Rock Materials category:
/MAT/LAW10 (DPRAG1)
/MAT/LAW21 (DPRAG)
/MAT/LAW24 (CONC)
/MAT/LAW81
could be used for coal, if the user has appropriate material properties. I have included the concrete material given as an example in Radioss help in the edited model attached below. Note the unit consistency is N, MPa, tonne, seconds.
3.** INCOMPATIBLE KINEMATIC CONDITIONS IN MODEL is not reported on my end. Given the boundary conditions, I do not see where the issue could be.
4. contact was modified
0 -
<?xml version="1.0" encoding="UTF-8"?>
Altair Forum User said:Hi,
I have made the following changes:
1. RBODY on element
master node of a rigid body should be independent (not connected to mesh). When creating rigids, make sure the primary node is set to calculate node. Pick this master node of rigid body for boundary condition 'Support'.
2. ** ERROR IN DRUCKER-PRAGER MATERIAL LAW 10 TENSILE BULK MODULUS IS LOWER OR EQUAL TO 0.
You have provided only density for this material, which is insufficient to run. Please search the literature for material properties of coal. All material laws in the Concrete and Rock Materials category:
/MAT/LAW10 (DPRAG1)
/MAT/LAW21 (DPRAG)
/MAT/LAW24 (CONC)
/MAT/LAW81
could be used for coal, if the user has appropriate material properties. I have included the concrete material given as an example in Radioss help in the edited model attached below. Note the unit consistency is N, MPa, tonne, seconds.
3.** INCOMPATIBLE KINEMATIC CONDITIONS IN MODEL is not reported on my end. Given the boundary conditions, I do not see where the issue could be.
4. contact was modified
Hi Ivan,
Thanks for the help. I tried to run the model and got a warning from RADIOSS saying there are initial penetrations in the interface. I realize this is now off-topic, however I was wondering if you might be able to help me in this regard? Running the penetration checker, I got the resulting image. I have attached the model I used. I changed a few things in the model that were causing errors, such as a missing material definition in the coal comp, and a surface inside the cylinder I forgot to remove.
There is no interference between the SPH elements and the surfs. It appears as though the rigids interfere with the surfaces, causing penetration? Running the simulation a warning is given about initial penetrations, then it never ends.
Any chance you would be able to help me with this?
Thanks for your time.
Best regards,
Ayman
0 -
You're welcome. There are a lot of penetrations in your models because contact parameter Gapmin (gap for impact activation) is set too high @10 (the model dimensions are 12*2m). Gapmin should be on the order of millimeters. Actually, rigids can not cause intersections and penetrations by themselves (only when attached to 1D, 2D or 3D elements they can penetrate, but even then penetrations are reported for components with Part card image). Sometimes even tool>Penetration Check in HyperMesh fails to find all and some are still reported in the starter out file. In this case use Hypercrash>quality>check all solver contact interfaces and set Fpenmax to 0.8
Try the attached solver deck:
0 -
Ivan,
Thanks again. I know I'm probably getting a little annoying by now, but I just want to make sure I understand everything as I am likely going to try to replicate this simulation on a much more complicated problem.
To be clear, in this case how did you fix the solver deck? Did you use Hypercrash>quality>check all solver contact interfaces and set Fpenmax to 0.8? I set Gapmin to the order of a few millimeters, and kept trying different incrementally smaller numbers and still got interference.
When I ran the solver deck you sent, the SPH particles are moving and impacting the walls of the tank, but inducing no stress/strain. What did I miss in this case? Is it because the time of the simulation is only fractions of a second?
Thanks for your help!
0 -
Try this example also from Radioss help.
<?xml version="1.0" encoding="UTF-8"?>
You can get the example model files from your installation directory for eg: (C:\Program Files\Altair\2017\demos\hwsolvers\radioss)
0 -
no problem, that's what forums are for, eh?
I used Hypercrash>quality>check all solver contact interfaces to automatically clear all penetrations (because Hypermesh does not find all).
Turns out my contact definitions were off, so it's better to go with the default. You can leave the Gapmin blank and the solver will automatically set the appropriate value.
Check the attached solver deck. Output requests for contact forces and pressures (ANIM/VECT/CONT & PCONT) are defined- I reckon you'll need them at some point.
0 -
(Writing this response in case there are future users trying to replicate this).
Ian,
Your model worked perfectly. I followed the steps as you described them and got the exact results.
You're a life saver! Thank you very much for your help!
0
