Hi Marcel Staubitzer , instead of distributing coupling, try using kinematic coupling. You can't define a distributed coupling with 1 to 1 connection.

Hi,

thanks for your reply. Does it also work with tie connector and how? Now I do use a beam model so I figurre that I have to connect my pointmass to the node in the middle of the beam, RP to node. But still I get these errors:

"Node set assembly__pickedset79 has not been defined

A concentrated load has been specified on node set assembly__pickedset79. This node set is not active in the model"

any suggests?

Thanks!

Hi Marcel Staubitzer , you are referring a node set named "assembly_pickedset79" in your model for applying a CLOAD but it is not defined in your model. Could you share the ".inp" file of this model? Check for it in the working directory.

Thanks.

Hi Pranoy Nair,

sorry I can't find the file anymore but I tried something else and it works now. Instead of using coupling or tie constraint I use MPC constraint with type beam (considering a beam as model type). I don't know why but this way made it possible to connect the RP applied with the pointmass and the middle node of the beam. (s. picture attached)

Calculated natural frequencies and static deflection is fine, but my initial problem remains. In the end I want to plot a diagramm for the max deflection resulting from centrifugal force in y-direction over rotational speed in x-direction. This should demonstrate the increasing deflection while approximating to the first mode. (s. png attached below)

I have already used a static analysis with rotational body force but that's only regarding to a certain rotation speed.

Hope, this is understandable..

additionaly:

The main problem is that the linked pointmass to the beam has no effect on the rotational body force analysis (even not on gravity load - static deflection was obtained by concentrated force). Also, when querying mass properties, there is no change of moment of intertia. Hope you can help.

Marcel Staubitzer Could you tell me more about the analysis procedure that you are using? Also, details on the time increment and the total time would be helpful. I have done similar analysis a couple of times, but I got the results what I expected.

Pranoy Nair ok what might be also interesting is that the beam is nearly mass less, only a concentrated point mass is defined in the middle. The problem is a rotational body force only could be applied to elements, wires etc. but not to nodes (=pointmass). Is there a way to apply a load by defining a function depending on the rotational frequency?

See my analysis procedure in the file. The step gravity uses a concentrated force, because a gravtiy load doesn't work with pointmass. Step zero just neutralizes the previous results. Total time of step rot. body force = 1sec.

Thanks in advance.

Marcel Staubitzer , Instead of Static analysis procedure, use *dynamic or *steady state dynamics procedure for your study. Static analysis wont consider the mass/inertia terms while solving, thus you won’t be able to capture the resonance at any critical speeds.

*Dynamic step (Implicit or explicit) which is a time domain approach can be used for your study; checking the response at a critical speed. But I would not count on the absolute values obtained from this procedures.

Instead, I would prefer *steady state dynamics (frequency domain) as it is quite faster and it seems like you’re interested in steady state response only. You can ramp the freq/RPM in both the cases.

Let me know if you’ve any more problems.

Thanks,

Pranoy Nair

Pranoy Nair Thanks, and sorry for the delay. I tried out the steady-state dynamics step, firstly using a CPL as load in the center of the beam. I defined its quadratically increasing amplitude (F=m*(r+e)*Omega²) in a table (out of excel) as expected from the resulting centrifugal force. The development of the graph looks fine but the values for U,V,A where not quite consistent to my analytic.

I am wondering how the applied load is working within the steady-state analysis.

Secondly I created a rotational body force in a further ssd step. The imbalance is connected by MPC-tie, node to node, to the center of the beam. Still, there is no deflection or any stresses.

Is there a way to define a (point)load as a function of rotational speed? It's quite nonsense to insert the explicit values for the centrifugal force which should be calculated actually by abaqus.

Hope, you can help. Thanks

Marcel

Marcel Staubitzer, For Steady-State Dynamics, yes! You need to generate the loads as per your requirement and apply in the SSD step. So for your case, If the beam is rotating about X-axis, along with the amplitude (mrw^2) details, capture the phase information as well to act along the Y and Z direction. This can be done by tweaking the real and imaginary part while calling in the CLOAD. The amplitude card (Frequency vs Force) can be called

Moreover, since SSD is a linear perturbation step, it will not carry forward the end results to the next SSD step. Each step is independent.

As you are comparing with the analytical calculation, make sure you are using the same damping value in either case. What value did you use for your analysis? This value does affect the response significantly at resonance.

***While doing any SSD analysis, the loading (as discussed previously) should be as close as you intend to simulate. In SSD Modal response, the equation of motions are solved at particular frequencies (info obtained from the *frequency step). If you want to solve the EOMs, at a set of frequencies of your choise, then you can do that as well.

For your case, this is what I would do.

1. Don't do Modal response. Delete the *Frequency Step.

2. Use *Steady State Dynamic, DIRECT

3. Create two Amplitude cards using *Amplitude for Frequency(Hz) vs Force (N). One for your load vector and other null vector.

4. In the *SSD step, use [*CLOAD, REAL & *CLOAD, IMAGINARY] to apply the in and out of phase component.

5. For example, if you created an amplitude card named "RAMP" which has the mrw^2 details, and create another amplitude card named "ZERO" which is nothing but a null vector, and if the beam is rotating about the X-Axis, use

*CLOAD, AMPLITUDE=RAMP, REAL,

Node no., 2,1

*CLOAD, amplitude=ZERO, IMAGINARY,

Node no., 2,1

*CLOAD, AMPLITUDE=ZERO, REAL,

Node no., 3,1

*CLOAD, amplitude=RAMP, IMAGINARY

Node no., 3,1.

Total, four CLOAD definition at the same node where you want to apply the imbalance. Assume some damping value (material or modal in consistent with the analytical calculations what you are doing). You are bound to get similar values from the simulation as the frequency response formulation is quite straightforward.

If you want Abaqus to calculate the required imbalance just by modelling an unbalanced mass/inertia, then that can be done using *Dynamic analysis. Use *Boundary, TYPE=VELOCITY and call the amplitude card (ramping speed) and apply this to beam supporting nodes. This way you don't need to explicitly give the load information. But as mentioned in my earlier post, the numerical damping affects the response amplitude.

You can also try looking at *modal dynamic which does transient modal dynamics (I have not explored much). Will need a frequency extraction step and time dependent loading data. Can carry forward the results from preceding step as well.

Thanks,

Pranoy Nair

Hi Pranoy Nair ,thanks a lot. I have a few questions:

• I created the CLOADs as you suggested. The calculation was successful, but why do you need a zero vector? The results still don't match with the analytics. Maybe the inp file helps - see below.
• What is EOM? ("If you want to solve the EOMs, ...")
• In my analytical calculation I use a damping value of 0.02 (Lehr's damping measure) What is the best way to add a similar damping in my model? Using ssd-direct I can't add damping within the step. So I can either add damping for my springs (dashpot coefficient) or for the material right? Reading the manual it says structural damping is suited for frequency domain dynamic procedures. So I put 0.02 there? I tried but no significant change of amplitude near natural frequency.
• Calculating the required imbalance just by modelling an unbalanced mass/inertia, which *Dynamic analysis do you propose? I tried dynamic explicit but it is very time consuming when I want to ramp the speed from zero to f_max in a realistic time intervall. What points (e.g. simple mesh) would you suggest to get a rough estimation using this procedure?

I appreciate your help,

Marcel

In addition:

I still prefer to let abaqus calculate the imbalance itself. Recently I tried a simple modalanalysis, with nearly massless material and a pointmass at the middle of the rotor (slightly set off the center). Now, how do I connect my pointmass to the rotor correctly? I've already created a surface in the middle to constrain the mass on it. I tried different constraints (see png). Errors as below appear

• three factorizations in a row failed
• The lanczos solver has failed to find all the eigenvalues

Changing the solver to subspace gives at least two frequencies but looses accuracy afterwards. Still, first value is quite correct.

Hi Marcel Staubitzer , sorry for the late reply.

1. I use the null vector just for my convenience to create the phase difference between the in-plane directions (Y and Z). You can resolve your vector as per some other random vectors just by switching the Re and Imag parts, but make sure that the magnitude is same as what you intend to have. I find it quite easy to do with null vectors.

2. By EOMs, I meant Equation of Motions. (Sorry)

3. If I assume correctly, Lehr's damping coefficient is velocity dependent and applies to the velocity term. The Structural damping coefficient (also known as loss factor) applies to the displacement term, thus making the stiffness a complex term, i.e. K+i(G). So, if you are using 0.02 as damping coefficient in your analytical calculations, the equivalent value for structural damping should be different. For a good guess, go ahead with a value of 0.04.

Before going to your 4th point, I have some questions regarding your modelling technique.

a. Why the beam is mass-less?

b. The unbalance mass, you modeled using solid elements? Use 1D Mass Element for this. Simply create a property using *MASS and assign the required value to it.

c. Why are the spring elements defined from the supported end to the center of the beam?

d. Why not use the beam elements instead of 3D elements? This would reduce the run time drastically.

4. Yeah, run time is the drawback of *Dynamic. Use Implicit dynamics, and control the speed ramp according to the modal content of your system. For Eg. if the *Frequency analysis gives 10Hz and 20Hz as first and second flexible modes, then those frequencies corresponds to 600 and 1200 RPM for the first order imbalance. So, I would define the speed ramp accordingly. Directly starting with an initial velocity of 550RPM (if no convergence issues), linearly increasing till 600RPM (hold for atleast 0.2 seconds) then ramp till 1200RPM (hold for atleast 0.1secs). My point is ramp faster through the region of no significance and hold at the speeds corresponding to the system's frequency content. Moreover, instead of using 3D elements, you can use beam elements and simply model the unbalance using 1D mass (offset by radius of the beam) (using 2 noded KINCOUP). This would reduce the run time significantly. Also, based on the frequency of interest, control the time increment step.

Let me know if I've not been efficient in making my point.

Hi Pranoy Nair ,never mind. Thanks for your time..

1. So, to get this right: I have calculated my centrifugal force analytically consisting of Re and Imag part (describing the y- and z-direction) which total amount is the resulting magnitude. Assuming there is no phase difference I only need to apply 2 Cloads, Imag and real -

*CLOAD, AMPLITUDE=RAMP, REAL,

Node no., 2,1 // = U2, Real=1, Imag=0i ?

*CLOAD, amplitude=RAMP, IMAGINARY

Node no., 3,1. // = U3, Real=0, Imag=1i ?

Now, as mentioned earlier, the amplitude card named "RAMP" has the mrw^2 values (total amount) which I would apply as shown above. But what do you think of this approach?

*CLOAD, AMPLITUDE=RAMP(real), REAL,

Node no., 2,1 // = U2, Real=1, Imag=0i

*CLOAD, amplitude=RAMP(imag), REAL

Node no., 3,1. // = U3, Real=1, Imag=0i

I get similar solutions but also varying orientation of the deflection.

2. Thanks ;)

3. But structural damping only within steady-state procedure right? Performing the *dynamic implicit procedure it was ignored. In my understanding I just need a global, overall damping factor. So during ssd modal analysis I use direct modal damping (0.02), in step ssd direct there is no damping available so I changed the damping properties of the material (structural =0.02) and in *dynamic, implicit I worked with Rayleigh damping (alpha_R = 0.05). Anyway the damping has no major effect below ~70% of first mode right?

Regarding my modelling technique:

a) Massless beauce firstly I want to compare my analytical modell with idealized pointmass.

b-d) ok, might be confusing - I am using two types of models: first is a 3D circular beam element, second (upper one) 3D body. The springs are connected to a center RP on the rotating axis which is coupled to the surface of the rotor.

But for now I am working with the beam element due to faster run time.

4. Good, first I wasn't aware of the needed transient oscillation. So I coupled the point mass to my beam (kinematic, all DOFs blocked) and applied a BC, velocity =

200rad/s, ramped from 0 to max in 0.5s and hold until 3s (see PNG below, y und z displacement displayed). As you can see the displacement is not converging as I would have expected.. I have no idea what might the reason why...

Thank you very much!

regards

Marcel

Hi Marcel Staubitzer

1. In case of your approach, both the loads along (Y and Z directions) are acting simultaneously with the same amplitude, which is generally not the case with the first order imbalance. For example, just imagine a rotating imbalance, at a certain point of time, the mass would try deflect the beam along Y axis and after completing a quarter rotation, the direction would be along Z axis acting with the same amplitude. Thus, in my case, I am trying to simulate the above scenario by explicitly giving the phase information of the rotating plane. But, in your case, since the phase difference is 0, its just a vector which is resultant of both the loads acting at 45 degrees (which is same as applying a load of 1.414 times the mrw2 value acting along Y or Z direction alone). Hope, I was able to clear my point, but I could be wrong too.

3. Yes, loss factor is valid only in SSD. The only form of material damping that you can provide is by using Rayleigh Coefficients in the material definition. For a structure like beam, I would agree with you.

4. So, did you apply the velocity BC to the Kincoup node which is attaching to the beam? If yes, could you try removing the BC from this node and apply to the end nodes of the beam (using DCOUP if beam modeled using 3D elements). Regarding, your displacement plot, at which node you're tracking the response? Also, check which node is dependent and independent in your Kincoup definition.

Regards,

Pranoy

Hi Pranoy Nair

1) Maybe you missunderstood me there. CLOAD 1 contains only the amplitude of the real force component, CLOAD 2 the imaginary. So the applied force in y-direction would be the cosinously part and in z-direction the sinously part ,thus its superposition gives the circulating, constant force. (see. F_Excel)

3) Well, now I just try a transient oscillation to see if the deflection is converging at a certain frequency. To do this I applied the sinously and cosinously working CF at the center of the beam so that the amplitude is constantly around 6 N.

Yet the beam is continuing oscillation (see the diagramm below). I have already experimented with rayleigh damping factors of alpha and beta but I have now idea how to determine them following these instructions:

https://classes.engineering.wustl.edu/2009/spring/mase5513/abaqus/docs/v6.6/books/usb/default.htm?startat=pt03ch06s03abo06.html

I am really wondering how this damping could work...

4) I applied the BC-velocity to the whole beam. Does it make a difference if I only select the end nodes of one side?

You mean checking the master-slave definition? My control point would be the node on the beam, the nodal surface is the RP pointmass.

Thanks again! You're my best hope

Regards

Marcel

Hi Marcel Staubitzer

1. My bad that I didn't see the definition of Real and Imag in Amplitude card itself. Yeah that should work similar to what I proposed.

3. So, here you gave sin/cos input with an amplitude of 6N? If yes, that's the solution I would expect and its pretty well a converged solution already (unless I'm missing something here). There's already enough damping present in the model. A rough value can be estimated by trial and error approach by suddenly making the load amplitude to 0 and your response will die out after some time. Using log-decrement method, you can estimate a rough value of the damping present in your system. I have not explored much about Rayleigh damping in simulations but the point is that solution looks neat to me. Is it possible to share the text data of the displacement response that you shared above?

4. Its better to apply the BC from where it is getting the power from. Applying to whole model does change the result as you are enforcing velocities to all the nodes.

Yes the master slave definition. Which is the master node?

Aha! We'll figure it out somehow but I am not your last hope :D

Thanks,

Pranoy