Modal analysis of a wood beam 2

[powerplay123]

Hi guys,

the following is my apdl code:

/PREP7

ET,1,SOLID45

MP,EX,1,0.789e9
MP,EY,1,1.365e9
MP,EZ,1,0.289e9

MP,GXY,1,0.053e9
MP,GYZ,1,0.474e9
MP,GXZ,1,0.543e9

MP,NUXY,1,.31
MP,NUXZ,1,.4
MP,NUYZ,1,.03

MP,dens,1,450

! MODELING
K,1,0,0,0
K,2,0.1,0,0
K,3,0.1,0.1,0
K,4,0,0.1,0

A,1,2,3,4

VEXT,1, , , , ,2

ESIZE,0.025
VMESH,1

KNODE,0,840
KNODE,0,524
KNODE,0,775
KNODE,0,459

L,9,10
L,11,12

DL,13, ,UX,
DL,13, ,UY,
DL,14, ,UX,
DL,14, ,UY,

DA,3, ,UX,
DA,3, ,UY,

F,26,FY,100
F,27,FY,100
F,28,FY,100
F,29,FY,100
F,30,FY,100

/SOLU
ANTY,MODAL
MODOPT,LANB,15,300,500,OFF,OFF

MXPAND,15,

SOLVE


1. First of all, ANSYS shows me this warning when i input the file: "The degree of freedom solution is not available. The PLDISP command is ignored."

I don't know how to fix that, so that I can look at the resulting mode shapes.

2. My second problem is, I want the forces at the nodes to hava an angle. In this case their showing in FY direction but i generally would like to keep the angle (which would be a combination of FY and FX) variable.

3. Also the external force (from point 2) is supposed to be the excitation with a certain frequency and not just constant without vibrating. However, i could not find the right command to do that.

I would be very grateful if you guys could help me with good advice.

Thanks in advance.

 

[kan123]

The default normal direction is the line between the 2 points of the contact element. But if your points are coincident, there is no line. That's why you have to explicitly define the normal direction.

The modal solutions are strictly linear. The eigensolution is found using a single stiffness matrix and a single mass matrix. This is basic theory.

For the static run, you apply your force load and verify that the response of the system is correct. Once that checks out, you can define a constant or time-varying force as the load in a transient solution. (Remember to have zero applied load for the first few time steps to allow the system to be in equilibrium before the load is applied.)

You can use as many *DO loops as you need. You can use geometry selects to restrict each component of nodes to a particular region.

 

[powerplay123]

I think its too complicated to specify the gap direction or normal directions (nx,ny,nz); instead, I tried to make sure that there is a geometric gap in the interface. So i set the gap 1e-5 in the real constant definition. However, I still get the error:

*** ERROR *** CP = 9.234 TIME= 23:38:20
The nodes of CONTAC52 element 1761 are coincident. Please define the
contact normal using real constant set 3.

It seems that I can't get around defining the gap direction. Generally this should be easy since there is only a displacement but no rotation from the global coordinates. But still I don't know how to specify that. I tried to get started with the approach that N=sqrt(Nx^2 + Ny^2 + Nz^2) but couldn't figure out the values of each component.

 

[kan123]

Setting a gap with the real constant won't change the location of the nodes, so that's why they are still coincident. (The gap only controls how much the nodes can move relative to one another before contact is made.)

If your table is aligned with the global coordinate system, then specifying the gap direction should be straight forward. For example, if the table surface is in the X-Y plane, then the normal direction is in the Z-axis and the real constant entries are NX,NY,NZ = 0,0,1.

 

[powerplay123]

Thanks very much! I could fix that and it works now.

But what I saw is that the *do loop from above sets contact elements that connect the nodes from the upper layer of the table with ALL overlying nodes of the beam.

Is that appropriate?

I was thinking the contact elements have to be set up solely between the table and the nodes that are directly above them. I assumed also that the relationship is 1:1 meaning that ONE node was supposed to contact only ONE other node from the other element type.

 

[kan123]

If you want to reduce the number of contact elements, you can use geometry selects to reduce the set of beam nodes that will have contact elements attached. However, having extra contact elements between pairs of nodes that will never come into contact shouldn't cause a problem because they will only transmit loads through soft springs. It is OK to have multiple nodes from one component attached to one node of another component -- this is common if the components have different mesh densities. (But if nodes are not coincident or do not line up normal to the contact plane, the real constant should be used to set the gap distance instead of relying on the node geometry.)

One other suggestion. Use a static load case to verify that the contact elements are oriented properly and the right ones make contact. The most common mistake is to have the elements defined backwards so that they open when they should close and vice versa.

 

[powerplay123]

OK I get your point. But if you take a look at the model (attached file) and let it animate you will see that it looks like even the nodes that are not in contact with the table get pulled. Or is this only the influence of the friction?

I generally wanted to the table element to act as constraint in negative y direction. But in the animation it appears as if the table impacts the movement of the beam in x and z direction as well.
The beam is supposed to constrain only the negative y direction. Assuming that there are no further constraints, the beam should still be able to move freely in x and z direction. Also the beam should have no constraints in positive y direction and be able to lift.
Do you think my parameters (ks, kn, redfact, MU) are not chosen correctly?

When I used the *do loop again it connected all nodes of the beam with the second rigid element. Again, I'm worried wether all the contact elements do not cause a problem.

 

[kan123]

You have KS=10e-12 which is not common if you are trying to incorporate friction. You might be better off using the default of KS=KN. Sometimes including friction can cause convergence problems for the gap elements (other times, it actually helps converge faster than the no-friction case).

Remember that when you do a modes solution, the gap elements are just treated as springs -- you won't get any bilinear behavior. When you do a static, you'll be able to see if the gaps are working properly.

 

[powerplay123]

I tried to do a statical analysis (please see the attached file). However, I dont know how to interpret this solution in regards to the point you made in your last comment.

Also, is there a way in ansys modelling to visualize the rigid links (the mpc184 parts)? Especially when you want to plot the results I would like them to be shown there to see explicitly how they influence the movement of the beam. It is also helpful when you are trying to show someone else the analysis who is not familiar with the code.

 

[kan123]

You can post-process the results to see which gaps closed (STAT output quantity) or look at separation and sliding displacements (USEP, UTY, and UTZ).

I haven't used MPC elements, so I don't know how they show up on plots. (I just explicitly define the constraint equations that I need.) Some elements that don't show up well in raster plots (/SHOW,,,0) sometimes show better in vector displays (/SHOW,,,1) or vice versa.

 

[powerplay123]

I'm struggling finding the right parameters for the contac52 contact elements!

I want kn, ks and possibly REDFACT to be determined so that the wooden beam is able to move (slide) on the steel desk and completely break the contact (lift off) without having penetration on the rigid steel desk.

If the parameters are too low the beam pretty much ignores the steel elements (e.g. the desk) when vibrating and penetrates into them. However, when the parameters are set too high, the beam element doesn't vibrate at all.

Generally the contact elements are supposed to only disable a deformation of the steel elements which function as some sort of "bearing" for the wooden element. Yet they beam shouldn't have any constraints in positive x,y and z directions caused by the contact elements.

Also I'm not sure about whether its okay that the steel element is connected with the inner nodes of the beam which it doesn't actually "touch".

(attached is the apdl code)

 

[kan123]

The attached file is for determining the modes. The contact elements loose their nonlinear capability in modal solutions -- they just act as springs. You need to do static runs to verify that the contact elements are working properly. Push the beam down onto the table and pull it up off the table. Once you verify that the contact elements open and close as expected, you can proceed to a transient solution with time-varying forces to excite your beam.

 

[powerplay123]

I made a static and transient analysis as you recommended.

However, I don't know how to interpret the results of the static analysis and see whether the contact elements are working properly or not. What I can definitely see is that the KN stiffness of the steel element underneath the wooden beam is too low and the beam can penetrate into it. (attached is the file)

The transient analysis with the time-varying forces seems to be wrong. I'm not sure if my time settings (start end and increment) are right and I incorporated the frequency (400Hz) appropriately into the code. Can you please take a look at it and tell me what is wrong?

 

[powerplay123]

static analysis

 

[kan123]

For your transient, I don't see any obvious problems except that your solution can't start at TIME=zero. I would recommend starting with a few time steps of zero load before launching your applied loads (because the solution at a given time makes use of the results at the previous time step).

To assess your static solution, you can see which contacts are closing by doing a post-processing plot. Use ETABLE to define STAT (NMISC,1) and plot with /PNUM,SVAL,1 so you can see the numbers.

(Since this thread has gotten long, you might have better luck getting responses from other users by starting a new one.)