×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Modal analysis of a wood beam
2

Modal analysis of a wood beam

Modal analysis of a wood beam

(OP)
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.

RE: Modal analysis of a wood beam

You do know that any external loads are irrelevant in an eigenvalue extraction? These can only be incorporated for a pre-stressed modal extraction which presumably from your code you're not undertaking.

To look at the mode shapes you will need to enter /post1 and open the results file, then select a set and type pldisp.


------------
See FAQ569-1083: Asking questions the smart way on Eng-Tips fora for details on how to make best use of Eng-Tips.com

RE: Modal analysis of a wood beam

(OP)
Thank you very much for your help so far.

I'm trying to simulate the vibration of the wooden beam which is excited by a planning tool with a particular Newton Force and a specific frequency. The excitation should take place at different places of the beam and also the experiment should be done for several beam geometries.

Now how can I implement that assuming the force has also an angle other than 90° (so it has both a x and y component)?

My other problem are the DOF constraints. For example: the beam is supposed to be on a machine tool table that constraints the beam in negative y-direction only. That is, the beam can swing and is free in positive y-direction.

What would be the code for that bottom area then?
"DA,3,UY," constraints all translation in y direction.

Thanks

RE: Modal analysis of a wood beam

As I said in my reply above, see the manual under Harmonic Analysis - make sure you read and understand all of it before continuing.


------------
See FAQ569-1083: Asking questions the smart way on Eng-Tips fora for details on how to make best use of Eng-Tips.com

RE: Modal analysis of a wood beam

If you want to have a restraint on the negative y-direction only, then you don't have a linear system and shouldn't be doing a modal frequency response or modal transient solution.  The way to incorporate the restaint is to include the table with contact elements between the beam and table.  Then you would do a direct transient solution.  You can apply any FX and FY you like as loads.

RE: Modal analysis of a wood beam

(OP)
Okay, so you are suggesting to position a fixed and inelastic element where the table would be and relate that element to the table somehow, right?

The way I make a element fixed would be through appropriate DOF contraints. So that would mean to constrain pretty much all DOF for the table element.

Do I have to put the beam in a relationship with the table when the table is already fixed and doesn't give the beam any freedom in that direction?

RE: Modal analysis of a wood beam

If the table is much stiffer than the beam, you can make it rigid if you like - restrain all of its degrees of freedom.  The relationship between the 2 components would be through contact elements which would be very stiff when the beam touches the table but have little or no stiffness when the beam is not in contact.  There are several types to choose from:  node-node, node-surface, surface-surface.

RE: Modal analysis of a wood beam

(OP)
I tried to set a table as a rigid element to constrain the beam in negative y-direction. I'd say its not a big challenge to implement a rigid body as the table with appropriate dof constraints, but the problem is to couple that rigid element adequately with the beam.

The table in the bottom is supposed to work pretty much as guidance (friction is neglected) that is rigid. However, the beam should be able to vibrate and wave in positive y-direction. But if i couple the nodes from the table with the beam (e.g. with a CE command), then the coincident nodes won't leave each other and stay coupled.

Then I'd would be exactly where I started by constraining transaltion in y-direction (positive and negative) for the bottom area.

How would you solve that problem. I really need some help.

Please find attached the sketch of this part of the problem.

RE: Modal analysis of a wood beam

Don't use constraint equations.  Use contact elements.  Start with the simplest: CONTAC12 for 2D or CONTAC52 for 3D.  KN should be relatively stiff in comparison to your beam material.  You may need Keyopt(3)=1 to maintain model continuity (soft spring stiffness controlled by REDFACT).

RE: Modal analysis of a wood beam

(OP)
I know my contact element definition must look as follows or very similar:

ET,2,CONTAC52
R,2,10e10, ,1,0, , ,
MP,MU,2,0
KEYOPT,2,3,1
KEYOPT,2,4,1    ! to have the gap size determined by the node location

also i defined an area which is supposed to represent the table. i set the density of that area to 0 to avoid that this table area contributes to the total mass.

and now the problem is to connect the appropriate nodes of the table and beam that are lying upon another. how do i do that with my contact elements???

thanks

RE: Modal analysis of a wood beam

If KN=10e10, you probably should use REDFACT because the default soft spring stiffness would then be 10e4.  If you have too many nodes to select the pairs by picking, you can form a component consisting of the nodes of the beam of interest.  Then write a macro to loop through those one at a time and find the nearest node of the table.  Since the resulting elements may not have their lines of action perpendicular to the table, you should use NX,NY,NZ to specify the element normal direction.

RE: Modal analysis of a wood beam

(OP)
kan123 man i'm really struggling with writing the macro with vba on excel. I generated a list (see attached file) but could not figure out a way to write the macro with vba even though i'm a good c++ programmer.

Please can anybody show me how to do that without using matlab? I'm really getting insane on that.

In this case only the y=0 nodes are of interest. The value should compare x and z values of nodes and write down the node numbers that contained x and z values that occured more than once.

RE: Modal analysis of a wood beam

I was just thinking of a macro within ANSYS using the APDL.  If you need to call it only once, you could use a *DO loop looking something like:

CMSEL,S,SET1_NODES
*GET,SET1_COUNT,NODE,0,COUNT
NODENUMB=0                  ! INITIALIZATION
*DO,I,1,SET1_COUNT,1
CMSEL,S,SET1_NODES
NODENUMB=NDNEXT(NODENUMB)   ! NEXT NODE IN SET 1
NSEL,R,NODE,,NODENUMB
CMSEL,A,SET2_NODES
NODE_J=NNEAR(NODENUMB)
E,NODENUMB,NODE_J
*ENDDO
ALLSEL

RE: Modal analysis of a wood beam

(OP)
Can u explain very briefly the function and how this macro works please? And where are the node numbers saved and how can i use those numbers DIRECTLY when I want to implement the contact elements....

I'm very sorry for all ur inconvenience but I really need some help to meet my deadline.

Thanks

RE: Modal analysis of a wood beam

Select the nodes of the beam (or the subset that could potentially come into contact with the table) and create a component for later use:
CM,SET1_NODES,NODE       ! SET OF BEAM NODES FOR CONTACT

Then do the same with the table nodes:
CM,SET2_NODES,NODE       ! SET OF TABLE NODES FOR CONTACT

The *DO loop will go through the set of beam nodes one by one (in node number order) and find the nearest table node.  The contact element is created with the chosen nodes.  You have to set the MAT, REAL, and TYPE before entering the loop.  Each command is described more fully in the Help Manual.
 

RE: Modal analysis of a wood beam

(OP)
OK I think I implemented everything so far but it doesnt run.

Here are the errors and warnings:
 *** WARNING ***                         CP =       3.469   TIME= 03:02:51
 Both solid model and finite element model boundary conditions have been
 applied to this model.  As solid loads are transferred to the nodes or  
 elements, they can overwrite directly applied loads.                    

 *** WARNING ***                         CP =       6.766   TIME= 03:03:51
 Both solid model and finite element model boundary conditions have been
 applied to this model.  As solid loads are transferred to the nodes or  
 elements, they can overwrite directly applied loads.                    

 *** WARNING ***                         CP =       7.047   TIME= 03:03:52
 Line 13 has no nodes associated with it.  Constraint not transferred.   

 *** WARNING ***                         CP =       7.047   TIME= 03:03:52
 Line 14 has no nodes associated with it.  Constraint not transferred.   

 *** ERROR ***                           CP =       7.297   TIME= 03:03:55
 The nodes of CONTAC52 element 1761 are coincident.  Please define the   
 contact normal using real constant set 3.

And please find attached the whole code including all the revised commands.

I'd appreciate every help.

RE: Modal analysis of a wood beam

(OP)
If the including the nnear function are the problem then i could basically do it without too.

Since I've determined the coincident nodes from ET1 and ET2 from my excel spreadsheet I could theoretically enter every contact pair manually if that would help.

RE: Modal analysis of a wood beam

The error is caused because you forgot to set the element orientation with NX, NY, NZ.  If the nodes are coincident, the program can't determine it automatically.  Since KN is so large, you should also specify REDFACT, maybe something like 10e-12 (or whatever will give you a "soft spring" on separation).  Be sure that KN isn't too large or you could have instability in a nonlinear solution.  It only needs to be 1 or 2 orders of magnitude stiffer than the elements making contact.

Be aware that if you do a modes solution, the bilinear contact elements will be treated as linear springs with the stiffness determined by their initial condition.  A nonlinear solution can only be done as a direct transient.  You can do a nonlinear static run first as a check.

RE: Modal analysis of a wood beam

(OP)
Okay I made some adjustments: As u suggested I defined redfact 10e-12 and also I reduced the value of kn to 10e6 to increase the stability. But how can i specify the normal direction at this point. I thought I can take the default values since there is table on which the beam is positioned is rigid. Or did i understood something wrong?


Regarding the nonlinear solution. The modal analysis is generally biliniear. How can I implement the static run and what does that physically mean.


Considering the macro above. Can I hypothetically use it more than once in the program when I lets say have the same contact elements problem on another side of the beam???


Thanks

RE: Modal analysis of a wood beam

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.

RE: Modal analysis of a wood beam

(OP)
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.

RE: Modal analysis of a wood beam

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.

RE: Modal analysis of a wood beam

(OP)
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.

RE: Modal analysis of a wood beam

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.

RE: Modal analysis of a wood beam

(OP)
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.

RE: Modal analysis of a wood beam

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.

RE: Modal analysis of a wood beam

(OP)
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.

RE: Modal analysis of a wood beam

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.

RE: Modal analysis of a wood beam

(OP)
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)

RE: Modal analysis of a wood beam

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.

RE: Modal analysis of a wood beam

(OP)
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?

 

RE: Modal analysis of a wood beam

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.)

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources