Is it a BUG in ANSYS 4

[thanhvan]

hi everyone,

I am not sure that pepole noticed this or not. That is the number of element for ANSYS model. I solve many problem by ANSYS and always found the same matter: the result will be fluctuated base on the number of elements, so what is it??

Let's take a simple example: I run the verification test case VM37 'Elongation of a slolid bar' available in ANSYS documents. The result is high accuracy 99.81% for stress solution with the number of element is 7. Then, I change the it into 70, and the results is 9800 (as compare with 8600 for previous solution) - means more than 10% diffence. So what happen?? I feel sock to see it, and also lost my belief. Please help me.
You can access the VM37 to check it by yourself. And please let me know if you found something.

Best wishes to all of you.

 

[strain2]

Hi

I ran this test case quite a long time before and found satisfactory results. However i havent tried it for greater number of elements (Mean refined meshing). I dont know the meshing technique you used for this problem. I guess if the number of elements are refined near ends the stresses are higher due to stress concentration at edges with boundary conditions (like fixed ends or load application points).

You can send me your meshed model.

STRAIN2

 

[thanhvan]

Hi strain,

Tell me how to send you the model (by command text file).

At first, I also thought like you, and also doubted about the aspect ratio. So I made the other model in which the aspec ration is 1 (element type 145, width=depth=length). I maintain this aspec ratio while increasing the number of element, but the result is as bad as previous solution. So, the aspect ratio here is not the main reason.

I have checked more model since I post my thread here, and all of them have the same problem.

Thanks so much for your concern, I hope we can understand this soon.

Regard.

 

[strain2]

Hi
You can send me the model by text file on my email below:

strain2@hotmail.com

What i am concerned in not aspect ratio but possibilty of too fine meshing (within acceptable aspect ratio), at boundary condition adges...which can result in higher stresses considering the area to be stress concentrated.

Anyways...u send and i'll check and will let you know if i can be of any help.

STRAIN2

 

[manoftheworld]

Hi thanvan and strain2,

I have your problems with belief as well, thanvan - the simple thing is when is a mesh fine or coarse enough when there are these big differences in the stress.

please discuss it in this thread (and not just one on one) to save my belief as well.

 

[thanhvan]

Hi mano,
I am still not sure about how fine the mesh is enough. If you have a glance throunh ANSYS document, you can see people want to use as least elements as possible. This is not reliable in some problem, esp. in fluid mechanic. And also in most of case I have test, I can not find what is the suitable one.
We need more people here. I hope.

 

[strain2]

Sorry for late reply. I am extremely busy in a design assingment of a process column (a huge one). I'm afraid i will not be able to continue with you guys this month.

Regards

STRAIN2

 

[DickButkus]

This is a very interesting problem. Although I am primarily an ABAQUS user, I believed ANSYS to be a good honest code also. Although I don't have access to ANSYS I would like to try and duplicate the problem in ABAQUS to see if it is an FEA artifact or code specific.

Best regards,
KF9RI

 

[thanhvan]

Thanks,

This is the code I am metioning. I change the number of division into 70 and having problem. You can check it first with number of division about 7 (the right solution- saying ANSYS Inc.)


A.37. VM37 Input Listing
/COM,ANSYS MEDIA REL. 60 (090601) REF. VERIF. MANUAL: REL. 60
/VERIFY,VM37
JPGPRF,500,100,1 ! MACRO TO SET PREFS FOR JPEG PLOTS
/SHOW,JPEG
/PREP7
smrt,off
/TITLE, VM37, ELONGATION OF A SOLID BAR
/COM INTROD. TO STRESS ANALYSIS, HARRIS, 1ST PRINTING, PAGE 237, PROB. 4
/COM USING 3-D STRUCTURAL SOLID ELEMENTS
ANTYPE,STATIC
ET,1,SOLID45
MP,EX,1,10.4E6
MP,NUXY,1,.3
K,1,1,,1 ! DEFINE KEYPOINTS
K,2,-1,,1
K,3,-1,,-1
K,4,1,,-1
K,5,.5,10,.5
K,6,-.5,10,.5
K,7,-.5,10,-.5
K,8,.5,10,-.5
V,1,2,3,4,5,6,7,8 ! DEFINE VOLUME
LSEL,S,LINE,,5,11,2 ! SELECT LINES
LESIZE,ALL,,,70 ! DEVIDE SELECTED LINES BY 7 DIVISIONS ==> I devide it by 70 devisions
LSEL,ALL ! SELECT ALL LINES
ESIZE,,1 ! USE 1 ELEMENT PER LINE DIVISION
/OUT,SCRATCH
VMESH,1 ! MESH THE VOLUME
/OUT
OUTPR,BASIC,ALL
NSEL,S,LOC,Y,0 ! APPLY BOUNDARY CONDITIONS AT THE BASE OF THE MODEL
D,ALL,ALL ! FIX ALL DEGREES OF FREEDOM AT SELECTED NODE SET
NSEL,ALL
NSEL,S,LOC,Y,10 ! APPLY LOAD ON FREE END OF THE MODEL
SF,,PRES,-10000
NSEL,ALL
FINISH
/SOLU
SOLVE

 

[juzz]

Hello, guys!

Do you think that ANSYS would put something strange in the verification cases?

Let's see the problem analytical. From Elasticity Theory we knew that where we have pressure boundary conditions the stress will be equal with pressure. So the maximum stresses (wich will be at the surface where pressure is applied) will be 10000 (psi, I believe). So when I have 70 divisions will be more accurate than I will have 7 divisions. In the vm case the value compared with analytical one is at the middle of the bar (4th element).

Conclusion: For this case more elements you have, more
accurate the answer at that surface will be.

More details: The element type used (it means SOLID45) has displacements varying linear along every axis. So the strain on every axis will be constant. By Hooke law the stresses are derived from strains so the stresses will be constant too on every elements. In our case will have a pure tension case so the stress that will interest us will be Sy. Being constant on element this stress will not represent the real case were the stress is varying by the law:

Sy = F/A

where

F = pressure*top area

A = quadratic function of y = r^2
r = r1 + (r2-r1)*y/L
where r1 and r2 are the edges of the sectional areas at the two limits of the beam and L is the length of the beam.

I hope that will be helpful for you,

Best regards,

Justin Onisoru
----------------------------
Scientific Researcher
Romanian Academy
Institute of Solid Mechanics
Ctin Mille 15
P. O. Box 1-863
Bucharest 010141
tel +40 21 3153810
fax +40 21 3157478
Romania
------------------------------

Additionally advice: The Finite Element Method is not about believing, it is about controlling. If you read carefuly the manuals of any FE Program (ANSYS, ABAQUS, NASTRAN etc.) you will see that the authors assume no responsability about the results of any analysis you made. So it will be your responsability to prove the valability of your results.