Bad Accuracy on displacement?

[transall]

Hello,

I'm doing some test with ansys,and I have problems with accuracy. The analysis is a simple bending of a circular beam (outer diam:20mm thickness:2mm) with a force of 2000N at one end and a 0 degree of freedom at the other end.
When I calculate analytically these problem I obtain a maximum displacement equal to 0.087mm. I try to solve the same problem with ansys using a beam 188 element after having defined circular section, and I obtain a maxium displacement of 0.11mm. We have a difference of 20% with the analytical solution!However, the maximum von mises equivalent constraint is accurate enough.
I tried different model and it is always the same result for the displacement.

The strange thing, it's when I do the same experimentation with a rectangular beam the displacement accuracy is good.

Could you explain me what happen?

Thank you for your help.

 

[meshparts]

I suppose you have have some errors in the definition of beam cross section data. Can you provide some code?

Regards,
Alex

 

[transall]

Alex,

I defined the beam cross dection via the GUI but the equivalent code for the circular beam is:

SECTYPE,1,BEAM,CTUBE
SECDATA,8e-3,10e-3,50

Regards,

Mickaël

 

[meshparts]

Okay... Have you also checked the beam with /eshape,1? Also check your hand calculations, boundary conditions...

I have also done some similar tests on a rectangular cross section with rounded corners. The tolerance was good...

Regards,
Alex

 

[transall]

I have checked the beam with shape checking. My hand calculation is good, i checked it. But i didn't use a rectangular beam but circular beam of 50m length (outer diam:20mm thickness:2mm).
If I use a rectangular beam the result is good, but not with a Ctube beam.

hand calculation

Y=(M.x^3)/EI
E=206000 Mpa
I= PI(D^4-d^4)/64=PI*(20^4-16^4)/64=4637
M=2000*50=1000 N/mm
Y=0.087mm

With ansys I found 0.11mm. For the boundary condition I use a 0 DOF constraint on one end node and a force of 2000N on the other end node.

Thank you for you help,

Mickaël

 

[meshparts]

Hi,

I used another formula:

Y=F*L^3/(24*EI)

Compared to your formula, you are using a Torque M instead of a Force F. And I have a factor of 1/24...

My hand calculations give me:

Y=0.11e-4 m

Ansys:

Y=0.11e-3 m

So I still have a factor of 10 but I must have a small mistake in my hand calculations or input code of ansys:

/prep7

mm=1/1000

et,1,beam188,0,1,0

mp,ex,1,206e9
mp,nuxy,1,0.3

sectype,1,beam,ctube
secdata,8*mm,10*mm,50

k,1,
k,2,50*mm

l,1,2

esize,,100
lmesh,all
eplo

d,1,all
f,2,fy,2000

/post1
uy=uy(2)

 

[transall]

How do you find this formula?

 

[transall]

I have done like following, and I think it's the good one (I have compared with the software called RDM6)

We start from Y''=-Mz/EIz
along the beam if x=0 where at the end DOF=0,we have Mz=F(x-L)
therefore Y''=F(L-x)/EIz
or Y'=F/EIz(Lx -x²/2)+C1
and Y=FL/EIz(Lx²/2-x^3/6)+C1x+C2
the initial conditions are y=0,dy/dx=0
Consequently,we have Y=FL/6EIz(3Lx²-x^3)
Ymax for x=L
=>Y=2FL^3/6EIz= FL^3/3EIz

=> in our case Ymax=0.087
I don't understand the value of ansys.

Thank you

Mickaël

 

[meshparts]

Hi Mickael,

I've verified your calculations, and they are correct. The I've changed the element type from beam188 to beam4 with following real constants:

! Area I_zz I_yy D D
r,1,113.0973e-6,4637e-12,4637e-12,20e-3,20e-3

The maximum displacement computed from Ansys is

Y_max=0.0872 mm

So we have absolute agreement with your hand calculations.

But I think, the results obtained with beam188 should be closer to reality. The difference between the to elements should be the formulation.

In the case of beam4 the cross sections of the beam remain perpendicular to the bending line. This is an idealization. I suppose the beam188 don't have this idealization... But I'm not sure of that...

The other formula I've used for my hand calculations I've found it with Google. Without derivation. If you compare my formula with your formula, you will see that they are almost identical. The only difference is a factor of 8.

I can't explain this at the moment. Perhaps other people on this forum can...

Regards,
Alex

 

[transall]

Hi Alex,

First of all, thank you for your help!

With beam 188, when you multiply the length by about 2.5 (freom 50mm to 120mm) the %error is divided by about 10 (from 20% to 2.2%).

Regards,
Mickaël

 

[transall]

Hi Alex,

you're right, I have made a calculation using Bernouilli theory and timoshenko theory, the results are:

Bernouilli: Ymax= 0.087 mm
Timoshenko: Ymax= 0.108 mm

That's why the results was different, my hand calculation was based on bernouilli theory, whereas my Ansys model was based on Timoshenko theory. And both theory give the same maximum equivalent Von Mises stress.

Thanks for all,

Mickaël