FEAP User Forum

FEAP => FEAPpv => Topic started by: agni_roni on March 13, 2018, 08:19:47 PM

Title: Output of stress values
Post by: agni_roni on March 13, 2018, 08:19:47 PM: Is there a possible way to obtain stress values in all directions at all nodes lying on a plane y=c?

Currently I am using : Stre,coor,2,0.02400000

But I am getting the following error :

Program received signal SIGBUS: Access to an undefined portion of a memory object.

Backtrace for this error:
#0 0x109202579
#1 0x109201945
#2 0x7fff6e6daf59
Bus error: 10

I have attached my input file. Thank you for your help!
Title: Re: Output of stress values
Post by: Prof. R.L. Taylor on March 13, 2018, 10:18:59 PM: 1. Your problem has a rigid body mode due to insufficient b.c.

2. ver8.5 output the surfaces for both the displacements and stresses (results are meaningless due to RBM).

What version of code are you using?

I do not think the iterative solver will converge for all plasticity solutions. You may need to check convergence. Also you need to incrent the loading with "time" steps for most plasticity problems
Title: Re: Output of stress values
Post by: agni_roni on March 13, 2018, 10:36:16 PM: Respected Professor,

I am in the process of checking for convergence.
Also, I am using VERSION: 4.1 Revision g. For the new version do I have to reinstall FEAPpv?

In this case, we do not have any rate dependency in our plasticity model (J2, isotropic hardening) which is why I am not incrementing the load. Do you think that approach is incorrect?

Thank you.
Title: Re: Output of stress values
Post by: FEAP_Admin on March 14, 2018, 01:11:23 AM: A couple of observations.

1) I do not think opti exists in FEAPpv, it is only in FEAP
2) As Prof. Taylor points out, your boundary conditions are wrong.
3) You always have to time step nonlinear problems!
4) Debug your problems on a smaller mesh

5) All that said, there does appear to be a problem with FEAPpv and stre,coor when the mesh size is large. We will have a look and let you know.
Title: Re: Output of stress values
Post by: Prof. R.L. Taylor on March 14, 2018, 07:46:10 AM: 1. In pmacr1.f around line 158 delete the statement: pzero(mr(np(60),numel)

2. In your data set a tolerance for the search, the default is much too large. I used 1.e-05
Title: Re: Output of stress values
Post by: FEAP_Admin on March 14, 2018, 01:10:58 PM: The git repository has been updated. To get a new copy

Code: [Select]
git clone https://github.com/sanjayg0/feappv
or

Code: [Select]
git pull
Title: Re: Output of stress values
Post by: Prof. R.L. Taylor on March 14, 2018, 06:29:18 PM: The previous report on the print stress was wrong. The array needs to be initialized. In an attempt to keep pointers the same as in FEAP the pointer for NSCR was moved from np(60) to np(207). This pointer is used to store error indicators for possible mesh refinement use. Thus, the correct initialization for the stress projection in module pmacr1.f of FEAPpv ver 4.1 is:

call pzero (hr(np(207)),numel)
followed by:
call pzero (hr(npnp), npstr*numnp)
call pzero (hr(nper), 8*numnp)
Title: Re: Output of stress values
Post by: agni_roni on March 14, 2018, 10:20:10 PM: Respected Professor and Admin,

I updated the codes but I still seem to get the similar error.

The new error is :
Program received signal SIGBUS: Access to an undefined portion of a memory object.

Backtrace for this error:
#0 0x105017579
#1 0x105016945
#2 0x7fff6e6daf59
Bus error: 10

I tried the Stress,Node option as well since I am using solid elements. It is also not working and I am getting the same error.
I have attached my code again with proper boundary conditions for your perusal.

Thank you.
Title: Re: Output of stress values
Post by: FEAP_Admin on March 15, 2018, 02:38:15 AM: The fix given should work (replace np(60) by np(207)). I have run your latest input file, and it runs just fine.

I suggest that you rebuild your code using the -g compile option and then run in the debugger (gdb) so that you can perform a stack trace
to identify the line causing the error.
Title: Re: Output of stress values
Post by: agni_roni on March 15, 2018, 02:50:13 AM: Respected Admin,

Yes, it does work now. I essentially reinstalled FEAPpv and then just pasted the pmacr1.f from your repository in the relevant folder. Works fine now.

Also thanks a lot for the advice on time incrementing my load.

By the way, optimize is working for me on FEAPpv along with the PCG solver. I will decide on using the PCG solver depending on the convergence analysis with and without the Iteration option.

Thank you for all your help, Professor Taylor and Admin.
Title: Re: Output of stress values
Post by: agni_roni on March 15, 2018, 03:17:24 PM: A quick follow-up question :

FEAPpv reports the stress values at the nodes in the following manner :
Node 1-Pr.Value 2-Pr.Value 3-Pr.Value 1-Pr.Angle
I_1 Value J_2 Value J_3 Value
1 Value 2 Value 3 Value 4 Value 5 Value 6 Value

Are the 1 Value, 2 Value, 3 Value, 4 Value, 5 Value, 6 Value the sigma_11,sigma_22,sigma_33,sigma_12,sigma_13,sigma_23 values respectively?

Thank you!
Title: Re: Output of stress values
Post by: Prof. R.L. Taylor on March 15, 2018, 05:53:47 PM: The values are in the same order as the element you use projects them. So if it is a solid element, then they are what you quote.