Learning Forum

[Zemos]

Hello,

In a modal analysis I want to create a lumped mass matrix for a cube and the corresponding stiffness matrix. The cube should initially only have nodes at the corners. 

My APDL command is:

/aux2 

file,file,full 

LUMPM,on,--,0

hbmat,massenmatrix,txt,,ascii,mass,no,yes 

hbmat,steifigkeitsmatrix,txt,,ascii,stiff,no,yes 

finish

 

 

Unfortunately I get 108 mass entries with 8 nodes, which is a consistent mass matrix, but should only get 24 entries (8 nodes x 3 degrees of freedom per node) 

 

I'm hoping someone can help me.

 

Regards

Zemos

[Wenlong]

Hi Zemos, 

Just curious, what if you try "LUMPM, on" instead of "LUMPM,on,--,0", I wonder if that "--" causes the problem. 

Regards,

Wenlong

 

[Zemos]

Hello Welong


Thank you for the answer . "LUMP,on" does not solve the problem.



I found out that the command "LUMP" runs under the process "Pre7". How to connect the command "LUMP" and the "HBMAT" command ?



Is it necessary to write several APDL commands and combine them ?



Regards

Zemos

[Wenlong]

Hi Zemos, 

If you are using MAPDL, you can simply add a new line "/prep7" before "LUMPM, ON". Below is an example:

/CLEAR
/FILNAME,myfile 
/TITLE, Dynamic Analysis
/PREP7

K,1,0,0    ! Enter keypoints
K,2,1,0

L,1,2    ! Create line

ET,1,BEAM3    ! Element type

R,1,0.0001,8.33e-10,0.01   ! Real Const: area,I,height

MP,EX,1,2.068e11   ! Young's modulus
MP,PRXY,1,0.33   ! Poisson's ratio
MP,DENS,1,7830   ! Density

LESIZE,ALL,,,10   ! Element size
LMESH,1    ! Mesh line
lumpm,on
FINISH
/SOLU

ANTYPE,2   ! Modal analysis
MODOPT,SUBSP,5   ! Subspace, 5 modes
EQSLV,FRONT   ! Frontal solver
MXPAND,5   ! Expand 5 modes

DK,1,ALL   ! Constrain keypoint one

SOLVE
FINISH

/AUX2
file, myfile, full
hbmat, massmatrix_no_lump, txt,,ASCII, mass, yes, yes
hbmat, massenmatrix,txt,,ascii,mass,no,yes 

 
!/POST1    ! List solutions
!SET,LIST
!
!SET,FIRST
!PLDISP    ! Display first mode shape
!
!ANMODE,10,0.5, ,0  ! Animate mode shape

For more readings, here is a relevant post: /forum/forums/topic/how-to-export-the-mass-matrix-from-superelements-substructure-file-sub/

Regards,

Wenlong

[Wenlong]

Hi Zemos, 

If you are using Mechanical, below is what you can do:

Regards,

Wenlong

 

[Zemos]

Hello Wenlong,

Thank you very much for the answer.  It works. Is there anything else I should have considered when creating the stiffness matrix, or does the concentrated mass matrix have no influence on the stiffness matrix?
Is it physically sensible to create a concentrated mass matrix for a cuboid ? Can you make a statement about this? I need the data from Ansys to process them in Matlab/Simulink. The advantage of the concentrated mass matrix is that the solver can work faster.

Thanks a lot
Zemos

 

 

[Wenlong]

Hi Zemos, 

Whether the mass matrix is lumped does not influence the stiffness matrix.

Which mass matrix to choose is a numerical choice. It does have its limitations (Ref:https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v201/en/ans_thry/thy_et2.html) But since you are using solid element, the following limitations shouldn't be a concern. 

12.5.3. Limitations of Lumped Mass Matrices

Lumped mass matrices have the following limitations:

1. 
   

   Elements containing both translational and rotational degrees of freedom will have mass contributions only for the translational degrees of freedom. Rotational degrees of freedom are included for SHELL181, BEAM188, BEAM189, SHELL208, SHELL209, SHELL281, PIPE288, PIPE289, and ELBOW290 (see Special Handling of Rotational Degrees of Freedom for details).

   
   


2. 
   

   Lumping, by its very nature, eliminates the concept of mass coupling between degrees of freedom. Therefore, the following restrictions exist:

   
   
   
   
   
   • 
     

     Lumping is not allowed for FLUID29, FLUID30, or FLUID38 elements.

     
     
   
   
   • 
     

     Lumping is not allowed for the mass matrix option of MATRIX27 elements if it is defined with nonzero off-diagonal terms.

     
     
   
   
   
   
   

Note that coupling due to constraint equations is always included.

Regards,

Wenlong

================ Note ====================

If you have trouble opening the links I attached, please see the first useful link below

 

 

---

Useful Links

---

• How to access Ansys Online Help Document


• How to show full resolution image


• How to use Google to search within Ansys Student Community

 

[Zemos]

Thank you very much for the answer.

 

I would like to press on my cube in Matlab/Simulink from above, but the knots should only move evenly in the Y direction. Therefore, in my understanding, the nodes need the same stiffness in the Y-direction. Is my project in ANSYS realizable via a boundary condition or similar?

Many thanks in advance.

 Regards

Zemos

 

 

[Wenlong]

Hello Zemos, 

In this case, you can apply a displacement control to the top face, in this way you will be constraining the nodes on the top face to move for the same amount. 

If you need to apply a force, you can apply a remote force and change the behavior to "coupled" (Ref: https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v201/en/wb_sim/ds_Geometry_Behavior.html)

Regards,

Wenlong

 

[Zemos]

Hello Wenlong,

Thank you very much for the answer. I hope it is not too much to ask, but could you explain or show me a small example of this?

[Wenlong]

Sure.

 

[Wenlong]

Let me expand more: For displacement control, you can simply insert a displacement boundary condition to the top face. 

For remote force:

A Remote Force is equivalent to a regular force load on a face or a force load on an edge, plus some moment.The advantage of using a remote force load is that you can directly specify the location in space from which the force originates. 

Another advantage is you can specify the behavior of the remote force, there are three behaviors "deformable", "rigid", and "coupled. 

To illustrate, we can imagine a remote force applied to a face, the location of the force is not on the center of the face.

For "Deformable", you can imagine the face as deformable and the area close to the force location will deform more. 

For "rigid", you can image the face as a rigid plate, it will not deform but it will rotate because the force is not applied to the face center. 

For "couple", every point on the face will be applied to the same amount of force. The geometry has the same DOF solution on its underlying nodes as the remote point location

Below is an illustration wiith behavior "coupled". 

Regards,

Wenlong

 

 

 

[Zemos]

Thanks for the answer.

My APDL command runs under a modal analysis, because I need the stiffness matrix and mass matrix in HB format for further investigations in Matlab/ Simulink.

 

I have not found your suggestion in a modal analysis. Basically, I want to allow the top of my cube to shift in the Y-direction in a modal analysis, but this shift must be uniform. 

 

In my opinion, this boundary condition should be triggered on the stiffness matrix so that if I load each node in the Simulink with the same force value, a uniform displacement of the top of the cube occurs.

 

I would like to apologize for the inconvenience.

Regards,

Zemos

[Wenlong]

Hi Zemos,

Oh sorry, I didn't realize you are talking about modal analysis. Then please ignore what I said before. In the modal analysis, you can use the "coupling" boundary condition or CP command in APDL. Please refer to the following links:

Coupling boundary condition in modal analysis

CP command in APDL

Regards,

Wenlong

 

[Zemos]

Hello Wenlong,
Unfortunately I can't access the information because I can't create an account in the Ansys Customer Portal.  I only have a student license. Can you provide me with the information in another way?

Regards,
Zemos

[Wenlong]

Hi Zemos,

Please see my first link below:

================ Note ====================

If you have trouble opening the links I attached, please see the first useful link below

 

 

---

Useful Links

---

• How to access Ansys Online Help Document


• How to show full resolution image


• How to use Google to search within Ansys Student Community

 

[Zemos]

Hello Wenlong,
thank you for all the tips.
I now have the following code in an APDl command:

/PREP7
LUMPM,on
CP,high,UY,NODE4,NODE5,NODE11,NODE14,NODE15,NODE24,NODE25,NODE26,NODE27

Ansys does not report an error message. Next, the HBMAT files are read into Matlab -> no error message.
Afterwards the cube is loaded with a force on the top side in Simulink.  The nodes of the top surface bend differently in the Y-direction anyway. In my opinion, because the stiffness matrix does not have the same numerical values everywhere in the Y-direction.
Did I use the command incorrectly?

The reason for the fact that the nodes of the upper side have to move equally far is due to the replica of the test stand. In the test stand the upper side of the cube sticks to a plate which presses the cube evenly together. The nodes of the upper side must deform evenly, otherwise they would lose contact with the plate.

Best Regards,
Zemos

 

[Wenlong]

Hello Zemos,

I see, so you are trying to output the stiffness and mass matrix after coupling and try to run it in a different solver. 

Please note that after assigning coupling, APDL does not change the corresponding items in the stiffness matrix to the same value, instead, it deletes the corresponding rows and columns whose DOFs are constrained. And that's why you couldn't find the same values. 

Please also note that after lines and rows are deleted, your output plot needs to be adjusted as well since the node numbering changes. If you are doing the whole process inside APDL you don't need to worry about that. But if you are doing calculation and post-processing using another solver, you will need to consider the mismatch. In my opinion, that is likely the cause you don't see uniform displacement on the top surface. 

Please see the following reference from Ansys online help document:

 Rows and columns corresponding to eliminated (slave) degrees of freedom from coupling and/or constraint equations (e.g., CE, CP commands) are also eliminated from the system of equations and are not written to the .MATRIX file. The DOFs that are eliminated from any coupling and/or constraint equations are determined internally by the solution code and may not match what you specified via the CE/CP (or similar) commands  

Regards,

Wenlong

 

 

[Wenlong]

Hello Zemos,

I see, so you are trying to output the stiffness and mass matrix after coupling and try to run it in a different solver. 

Please note that after assigning coupling, APDL does not change the corresponding items in the stiffness matrix to the same value, instead, it deletes the corresponding rows and columns whose DOFs are constrained. And that's why you couldn't find the same values. 

Please also note that after lines and rows are deleted, your output plot needs to be adjusted as well since the node numbering changes. If you are doing the whole process inside APDL you don't need to worry about that. But if you are doing calculation and post-processing using another solver, you will need to consider the mismatch. In my opinion, that is likely the cause you don't see uniform displacement on the top surface. 

Please see the following reference from Ansys online help document:

 Rows and columns corresponding to eliminated (slave) degrees of freedom from coupling and/or constraint equations (e.g., CE, CP commands) are also eliminated from the system of equations and are not written to the .MATRIX file. The DOFs that are eliminated from any coupling and/or constraint equations are determined internally by the solution code and may not match what you specified via the CE/CP (or similar) commands  

Regards,

Wenlong

 

 

 

From