error in modal analisys

[marcoqc2012]

Dear friends

i try resolve whith manual calculations a simple cantilever beam

!--------

b= 3cm

h= 1cm

l = 100 cm = 1 m

whith the simple formula W=sqr(k/m)

angular frecuency = 25.6 rad/s

natural frecuency = 4.07 hz

the material is steel astm a36 E=2100000 kc/cm2

when i try this model in inventor and mechanical give me other results

please your helps

thank

[AstroJohnPE]

Hi marcoqc2012,

Using your values and a density for steel, I calculate a natural frequency of 8.3 Hz.

What result does Inventor give?

What result does Simulation Mechanical give?

[marcoqc2012]

thanks dear friend

attach the sample in diferents software

sap2000 (material using databe default) F = 4.01 HZ

robot (material using databe default) F = 4.01

i using inventor 2015 and simulation 2015

thanks

[marcoqc2012]

sap and robot

[AstroJohnPE]

I've determined the problem: you made a mistake. Of course, we cannot determine what the mistake is because you did not include any results from Simulation Mechanical, like the frequency result, the displaced shape, element type, constraints, and so on. Please check the dimensions in your original post and compare your Simulation Mechanical model to those. If you still have the wrong results, I suggest that you attach your hand calculation and archive of your Simulation Mechanical model. (Search the discussion board for the thread "Create, Post, or Provide an Archive of your model").

I did two analyses in Simulation Mechanical. Using the dimensions given in your original post, beam elements give a result of 8.14 Hz, and brick elements give a result of 8.20 Hz. These match my hand calculation of 8.3 Hz using the formula for a cantilever beam with a uniform load (the weight of the beam) given in Roark's Formulas for Stress and Strain.

[marcoqc2012]

dear thanks for your time

sorry for tha bad english, i from peru

last night i try made a phisical model in my house whit this dimentions:

b = 2.54 cm = 1 in

h = 0.3 cm = 3mm = 0.125 in

large = 1m = 100 cm

hand calculations:

w = 7.68 rad/s

f = 1.22 hz 

phisical test = near 1 hz

1. ANALISYS WHITH AUTODESK ROBOT 2015 (f = 1.2 hz)

2. ANALISYS WHITH SAP2000 V 17 (f = 1.2 hz)

3. ANALISYS WHITH AUTODESK SIMULATION 2015 (f = 2.4 hz)

Attach files in robot, sap and simulation

i work in autodesk atc in peru (semco), please help me.

Thanks

[AstroJohnPE]

Hi marcoqc2012,

Your English is fine, so do not worry about that.

Your situation is very bizarre. I do not see any problems with the setup of the Simulation Mechanical model. My hand calculations for this new geometry give a frequency of 2.44 Hz which matches the Simulation Mechanical results! Please check my hand calculations to see if I have made a mistake. (I can understand a modeling error if wrong material properties are entered by hand or some other setup problem occurs, but it is hard to say that the physical test is giving wrong answers!!!)

L = length = 1 m

A = area = (0.0254 m)*(0.003 m) = 7.62E-5 m^2

m = mass per unit length = A*(7855 kg/m^3) = 0.5986 kg/m

I = area moment of inertia = (1/12)(0.0254 m)*(0.003 m)^3 = 5.715E-11 m^4

E = modulus of elasiciticy = 2E11 N/m^2

omega = natural frequency = (3.515/L^2)*sqrt(E*I/m) = 15.36 rad/sec. (I checked the units, and they are dimensionally consistent.)

f = natural frequency = omega/2/pi = 2.44 Hz

The above formula for the natural frequency (omega) is from my vibrations text book, and it agrees with the formula from Roark's Formulas for Stress and Strain.

My guess is that there is a problem with the units somewhere.

[marcoqc2012]

Dear friend, thank you very much for your time

I believe that the problem is in defining in the software the procedence of the mass, in sap and robot i define that.

attach hand calculations

[marcoqc2012]

i remember tree years ago, i resolve this problem whit other version i thing algor 2011

the results corresponded whith algor , sap and robot, Inclusively comsol.

that problem.....

a hug from peru.

[AstroJohnPE]

Hi,

I think your hand calculations are for a massless beam with a weight on the end. When I use an equation from Roark's for that type of geometry, I calculate a frequency of 1.21 Hz, and this matches your hand calculations. When you created the analysis in Robot and SAP, did you apply the mass (weight) at the end of the beam, or is it distributed along the length of the beam?

The Simulation Mechanical analysis distributes the mass along the length of the beam (area * density), so the answer of 2.44 Hz is correct for that input. I'm sure that you would get close to 1.2 Hz if you were to change the model to simulate your hand calculations by doing the following:

• edit the material
• change the density to 0 or a very small value, and OK the changes. (I don't know if the analysis will run with a density of 0, so that's why I suggest a small value so that the total mass of the beam is approximately 0.)
• select the vertices on the free end of the beam
• add a nodal weight. The value would be 0.59 kg/number of nodes. (The number of nodes is shown in the title of the dialog.)
• run the analysis.

Mystery hopefully solved.

[marcoqc2012]

Dear friend in robot and sap the mass is computing directly in the mass matriz when the user choose the procedence.

in this case the mass is from selftweight

when i create the model i don't  assign additional mass in begin and end of the beam, the software computing Automatically the mass.

He worries me her no representation of the physical phenomenon

I am recording a video of the experiment.

Greetings

thank you

[avijeetsuryavanshi]

it will give approximatevsolution nd we will try achive close result to analytical solution.