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.
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
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
------------
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
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
------------
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
RE: Modal analysis of a wood beam
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
RE: Modal analysis of a wood 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
RE: Modal analysis of a wood beam
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
RE: Modal analysis of a wood beam
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
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
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
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
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
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
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
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 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
*** 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
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
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
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
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
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
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
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
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
RE: Modal analysis of a wood beam
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
RE: Modal analysis of a wood beam
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.)