An exclusive raffle opportunity for active members like you! Complete your profile, answer questions and get your first accepted badge to enter the raffle.
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.
Please let us know what type of contact interface you have in your model,
Dear All,
I am getting the same error after imposing the constant time step . I have used Type 7 contact in my model.
0.9 3e-5
Initial time step was 1.03 e-07
Thanks
RAM
Please change the Stfac to 1 in interface and try running the analysis.
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,
Do you have any type 2 interface in the model?
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.
whether it is a rigid body master node (1068085)?.
No it is not rigid body master node.
<?xml version="1.0" encoding="UTF-8"?>
Can you share the model files (starter and engine) to my dropbox link?
I had dropped the model in your drop box.
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.
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?
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
.
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.
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.
Thanks for your valuable support.
Regards
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?
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.
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
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.
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 .
Dear Ram,
Make IDROT=1 in /IOFLAG and try running the analysis.Please check the results then.
Analysis>>Control Cards>>IOFlagCard
