Negative stiffness node error

gopal_rathore
gopal_rathore Altair Community Member
edited October 2020 in Community Q&A

Hi,

I am getting a negative stiffness node error in the radioss run after adding constant time step :

/DT/NODA/CST

0.9 6E-8

 

Initial time step was 5.84 e-07 

There are no contacts at these nodes.

Tagged:

Answers

  • Altair Forum User
    Altair Forum User
    Altair Employee
    edited October 2015

    Hi,

     

    Please let us know what type of contact interface you have in your model,

  • RAMGANESH
    RAMGANESH Altair Community Member
    edited July 2016

    Dear All,

     

    I am getting the same error after imposing the constant time step . I have used Type 7  contact in my model.

     

    /DT/NODA/CST

     

    0.9 3e-5

     

     

     

    Initial time step was 1.03 e-07 

     

    Thanks

    RAM

  • Altair Forum User
    Altair Forum User
    Altair Employee
    edited July 2016

    Please change the Stfac to 1 in interface and try running the analysis.

  • RAMGANESH
    RAMGANESH Altair Community Member
    edited July 2016

    Dear George ,

     

    Same error occurs again after changing the STfac to 1 in interface.

     

    ROOT: ssc93  RESTART: 0001
     NUMBER OF HMPP PROCESSES     2
     12/07/2016
      **ERROR : NEGATIVE STIFFNESS NODE     1068085
      **ERROR : NEGATIVE STIFFNESS NODE     1068085
     NC=       0 T= 0.0000E+00 DT= 1.0368E-07 ERR=  0.0% DM/M= 8.3687E+01
         ANIMATION FILE: ssc93A001 WRITTEN
         RESTART FILES: ssc93_0001_[0001-0001].rst WRITTEN

                               ** CPU USER TIME **

     #PROC  CONT.SORT  CONT. F   ELEMENT  KIN.COND.  INTEGR.    I/O     TASK0     ASSEMB.   RESOL
       1   .1016E+01 .0000E+00 .1359E+01 .3125E-01 .9375E-01 .1797E+01 .1250E+00 .3125E-01 .2169E+02

                       ** CUMULATIVE CPU TIME SUMMARY **

     CONTACT SORTING............: .1016E+01     4.68 %
     CONTACT FORCES.............: .0000E+00     0.00 %
     ELEMENT FORCES.............: .1359E+01     6.27 %
     KINEMATIC COND.............: .3125E-01     0.14 %

     

     

    regards

    RAM

  • Altair Forum User
    Altair Forum User
    Altair Employee
    edited July 2016

    Ram,

    Do you have any type 2 interface in the model?

  • RAMGANESH
    RAMGANESH Altair Community Member
    edited July 2016

    Dear George,

     

    I dont have Type 2 interface in my model.

     

    I have Two Type 7 interface in my model.

     

    one is self contact and other is contact between model and ground.

     

    regards

    RAM

  • Altair Forum User
    Altair Forum User
    Altair Employee
    edited July 2016

    Ram,

     whether it is a rigid body master node (1068085)?. 

  • RAMGANESH
    RAMGANESH Altair Community Member
    edited July 2016

    No it is not rigid body master node.

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

  • Altair Forum User
    Altair Forum User
    Altair Employee
    edited July 2016

    Can you share the model files (starter and engine) to my dropbox link?

  • RAMGANESH
    RAMGANESH Altair Community Member
    edited July 2016

    Dear George,

     

    I had dropped the model in your drop box.

     

    Thanks

    RAM 

  • Altair Forum User
    Altair Forum User
    Altair Employee
    edited July 2016

    Ram,

    It is running in HW 14.0 version. Please upgrade your HW version and try running it.

    Please clear the penetrations in the model and also impose a fair time step. In the current file mass error is too high and it will terminate the run quickly. So impose a good time step in the model.

     

  • RAMGANESH
    RAMGANESH Altair Community Member
    edited July 2016

    Dear George,

     

    Thanks for your support.

     

    Fair time step means?

     

    Element size in my model is 10mm & 15mm (Majority)

     

    Also explain about AMS and how to impose it?

     

    Thanks

    RAM

     

  • Altair Forum User
    Altair Forum User
    Altair Employee
    edited July 2016

    Ram,

    The time step now imposed is much higher and so the mass added is is also higher. Try with a smaller value which will not add too much mass to the model.

     

    When you impose /AMS (Advanced Mass Scaling) in the model a non physical mass is added to a structure in order to achieve a larger explicit time step. And so. no mass is actually added to the system while solving. Choose a minimum time step, Tmin, from 10 to 20 times than the one used in /DT/NODA/CST. Tsca used is 0.67 for /AMS.

    When /DT/AMS is present in RADIOSS Engine Input, option /AMS is mandatory in RADIOSS Starter Input file

    The format for input is     /DT/AMS

                                               Tsca Tmin

    In Help Menu, please see the  Example 44- Blow Molding with AMS.

    For more info on time step control without compromising the accuracy, please visit the link below:

    http://www.altairhyperworks.com/html/en-US/rl/RADIOSS_Simulation_91212.htm

    .

  • RAMGANESH
    RAMGANESH Altair Community Member
    edited July 2016

    Dear George,

     

    After imposing AMS the model is running fine without any error.

     

    I had given   /DT/AMS

    Iflag - 1

    Tsca - .67

    Tmin - 3 e-7

     

    Whether there is any standard for calculating the Tmin for AMS.

     

    Thanks

    RAM

  • Altair Forum User
    Altair Forum User
    Altair Employee
    edited July 2016

    Ram,

    There is no standard rule but as a fair practice we can tell,

    Any targeted model for AMS application should run first in /DT/NODA/CST with a reasonable energy error and acceptable added mass along its simulation time.Computational convergence and accurate results can be obtained by choosing a minimum time step, Tmin, from 10 to 20 times than the one used in /DT/NODA/CST. 

    If the Tmin input is more the AMS job may either fail or diverge, most likely with an error message.

  • RAMGANESH
    RAMGANESH Altair Community Member
    edited July 2016

    Dear George,

     

    Thanks for your valuable  support. 

     

    Regards

    RAM

  • RAMGANESH
    RAMGANESH Altair Community Member
    edited July 2016

    Dear George,

     

    In my model i have given initial velocity about y axis , but in the result in hyperview it shows zero.

     

    since gravity also comes into the account ,it is difficult to find whether the solver took the velocity or not.  

     

    How can we check whether the solver takes that initial velocity or not?

     

    Thanks

    RAM

     

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

  • Altair Forum User
    Altair Forum User
    Altair Employee
    edited July 2016

    Ram,

    I dont think we have such an option available. But the solver will take the loads applied by the user, if there are no kinematic constraints.

  • RAMGANESH
    RAMGANESH Altair Community Member
    edited July 2016

    Dear George ,

     

    I have recreated the initial velocity about an axis but the solver is not taking the velocity which i had applied .

     

    In results it shows zero value.

     

    Kindly provide your guidelines 

     

    Thanks

    RAM

  • Altair Forum User
    Altair Forum User
    Altair Employee
    edited July 2016

    Ram,

    Ensure you have applied the loads correctly to the model. If any rigid bodies are there, ensure the load is applied in the master node also.

    Make sure that the kinematic constraints also does not violate the loads applied.

  • RAMGANESH
    RAMGANESH Altair Community Member
    edited July 2016

    Dear George,

     

    I have checked the model and recreated the initial velocity but can't able to identify the error.please check my model which i had shared in your dropbox and let me know the error .

     

    Thanks

    RAM

  • Altair Forum User
    Altair Forum User
    Altair Employee
    edited July 2016

    Dear Ram,

    Make IDROT=1 in /IOFLAG and try running the analysis.Please check the results then.

    Analysis>>Control Cards>>IOFlagCard

    <?xml version="1.0" encoding="UTF-8"?>Capture2.JPG

Categories