It is sometimes useful to extract the mass and stiffness matrix from Ansys.

*SMAT, MatK, D, IMPORT, FULL, file.full, STIFF

*PRINT, matk, matk, txt

Exporting mass matrix would be similar:

*SMAT, MatM, D, import, full, file.full, MASS

The above script uses APDL Math to get the job done. (Please see previous post for another example). The ordering of the matrix is unfortunately not concurrently exported. To verify the sequencing is as expected, we will work to replicate a truss example in the Finite Element Trusses course notes by Bob Greenlee.

Script to create model:

/prep7

!! Creates Model to reflect course notes

! Properties

et,1,1

mp, ex, 1, 29.5e6

r, 1, 1

! Geometry

n,1 $ n,2, 40 $ n,3, 40, 30 $ n,4, 0, 30

e,1,2 $ e,2,3 $ e,1,3 $ e,3,4

! Boundary Conditions

d,1,ux,0 $ d,1,uy,0

d,2,uy,0

d,4,ux,0 $ d,4,uy,0

f,2,fx,20e3

f,3,fy,-25e3

! solves

/solu

eqslv, sparse

wrfull, 1

solve

finish

save

With the

! Gets Stiffness Matrix

*SMAT, MatK, D, import, full, file.full, stiff

*SMAT, Nod2Bcs, D, import, full, file.full,NOD2BCS

*print, MatK, matk.txt ! Exports Stiffness to Text File

*export, MatK, mmf, matkMMF.txt ! Exports Stiffness as MMF format

Here's the MatK matrix printed out. Note it is is both sparse and assumed symmetric.

This compares favorably to the course notes:

Despite having 4 nodes with UX and UY (total of 8 DOF), there are only 3 DOF here because the boundary condition equations were removed leaving DOF # 3, 5 and 6. In this case the ordering was in sequence but the Degree of Freedom Ordering Documentation states that the ordering may be optimized for solving.

The node numbering we use in APDL is

*VEC,MapForward,I,IMPORT,FULL,file.full,FORWARD

*dim, Xint,, MAPFORWARD_ROWDIM*MAPFORWARD_NUMDOF

cto=0

*do, EUnodeNumber, 1, MAPFORWARD_ROWDIM

*do, dofdir, 1, MAPFORWARD_NUMDOF

j = MapForward(EUnodeNumber)

cto=cto+1

Xint(cto) = (j-1)*MAPFORWARD_NUMDOF+dofdir

*enddo

*enddo

Next, another mapping vector was multiplied to get

*VEC, Xxint, d, import, apdl, Xint ! from previous equivalence

*MULT, Nod2Bcs,, Xxint,, Xbcs ! X of BCS ordering

*PRINT, Xbcs ! Indexing of BCS (see output window)

That gets us the Xbcs ordering (Figure 4) which reflects the DOF subscript in Figure 3.

To continue solving the FE problem in APDL Math, the equations are solved with results identical to the course notes:

*VEC,vRHS,D,IMPORT,FULL,file.full,RHS

*LSENGINE,BCS,MyBcsSolver,MatK

*LSFACTOR,MyBcsSolver

*DMAT,VecX,D,COPY,vRHS

*LSBAC,MyBcsSolver,vRHS,VecX

*PRINT, VecX

APDL Math allows us to manipulate the internal matrix and vectors quite effectively once some familiarity was established. Depending on the task at hand, it may be worth while doing the calculation inside Ansys with APDL Math instead of exporting and calculating it externally in Matlab/Octave or Python etc.

Speaking of Python, I came across pyansys by Alex Kaszynski which exports the K and M matrix and it's corresponding node and degree of freedom. Unfortunately my attempt had an error of ValueError. If anyone else is able to get it to work, please let me know in the comments section. Thanks!

APDL script of the above project: WriteStiffness.inp

*SMAT, MatK, D, IMPORT, FULL, file.full, STIFF

*PRINT, matk, matk, txt

Exporting mass matrix would be similar:

*SMAT, MatM, D, import, full, file.full, MASS

The above script uses APDL Math to get the job done. (Please see previous post for another example). The ordering of the matrix is unfortunately not concurrently exported. To verify the sequencing is as expected, we will work to replicate a truss example in the Finite Element Trusses course notes by Bob Greenlee.

Figure 1: Truss Problem Setup

**Model Creation**Script to create model:

/prep7

!! Creates Model to reflect course notes

! Properties

et,1,1

mp, ex, 1, 29.5e6

r, 1, 1

! Geometry

n,1 $ n,2, 40 $ n,3, 40, 30 $ n,4, 0, 30

e,1,2 $ e,2,3 $ e,1,3 $ e,3,4

! Boundary Conditions

d,1,ux,0 $ d,1,uy,0

d,2,uy,0

d,4,ux,0 $ d,4,uy,0

f,2,fx,20e3

f,3,fy,-25e3

! solves

/solu

eqslv, sparse

wrfull, 1

solve

finish

save

**Extract & Export Stiffness Matrix**With the

**file.full**file of the FEM model created, let's now export the stiffness matrix to both a text file and MMF file format.! Gets Stiffness Matrix

*SMAT, MatK, D, import, full, file.full, stiff

*SMAT, Nod2Bcs, D, import, full, file.full,NOD2BCS

*print, MatK, matk.txt ! Exports Stiffness to Text File

*export, MatK, mmf, matkMMF.txt ! Exports Stiffness as MMF format

Figure 2: Stiffness Matrix

This compares favorably to the course notes:

Figure 3: Course Notes Values

**DOF Ordering**Despite having 4 nodes with UX and UY (total of 8 DOF), there are only 3 DOF here because the boundary condition equations were removed leaving DOF # 3, 5 and 6. In this case the ordering was in sequence but the Degree of Freedom Ordering Documentation states that the ordering may be optimized for solving.

The node numbering we use in APDL is

**User Ordering.**To convert that to**Internal Ordering**that removes unused node number and optimized reordering, we use the FORWARD nodal vector mapping. Here's my interpretation of mapping the 4 sequential nodes into**Internal Ordering**.*VEC,MapForward,I,IMPORT,FULL,file.full,FORWARD

*dim, Xint,, MAPFORWARD_ROWDIM*MAPFORWARD_NUMDOF

cto=0

*do, EUnodeNumber, 1, MAPFORWARD_ROWDIM

*do, dofdir, 1, MAPFORWARD_NUMDOF

j = MapForward(EUnodeNumber)

cto=cto+1

Xint(cto) = (j-1)*MAPFORWARD_NUMDOF+dofdir

*enddo

*enddo

Next, another mapping vector was multiplied to get

**BCS Ordering**from**Internal Ordering**.*VEC, Xxint, d, import, apdl, Xint ! from previous equivalence

*MULT, Nod2Bcs,, Xxint,, Xbcs ! X of BCS ordering

*PRINT, Xbcs ! Indexing of BCS (see output window)

That gets us the Xbcs ordering (Figure 4) which reflects the DOF subscript in Figure 3.

Figure 4: Xbcs index

**Solving for Displacements**To continue solving the FE problem in APDL Math, the equations are solved with results identical to the course notes:

*VEC,vRHS,D,IMPORT,FULL,file.full,RHS

*LSENGINE,BCS,MyBcsSolver,MatK

*LSFACTOR,MyBcsSolver

*DMAT,VecX,D,COPY,vRHS

*LSBAC,MyBcsSolver,vRHS,VecX

*PRINT, VecX

Figure 5: Solved Displacement

**Conclusions**APDL Math allows us to manipulate the internal matrix and vectors quite effectively once some familiarity was established. Depending on the task at hand, it may be worth while doing the calculation inside Ansys with APDL Math instead of exporting and calculating it externally in Matlab/Octave or Python etc.

Speaking of Python, I came across pyansys by Alex Kaszynski which exports the K and M matrix and it's corresponding node and degree of freedom. Unfortunately my attempt had an error of ValueError. If anyone else is able to get it to work, please let me know in the comments section. Thanks!

**Addendum**APDL script of the above project: WriteStiffness.inp

pyansys seems to be very limited at this stage but I do realize it's future potential. It can only deal with the following element types- '45', '95', '185', '186', '92', '187'

ReplyDeleteThanks Abhijeet! That's good to know. Could you share a link that lists it's limitation?

DeleteCheers,

Jason

I was going through the pyansys python code listed at github.

DeleteThanks for the pointer. Here is the link if others are interested:

Deletehttps://github.com/akaszynski/pyansys/blob/61790110ed14a69403457bc6ae26b04de55424b0/pyansys/archive_reader.py

Hi Jason,

ReplyDeleteDo you have an example how APDL math can be use for parameter sensitivity study of a model ?

Thanks

Here is a not-so-good example for modal sensitivity: https://www.ansystips.com/2017/06/apdl-math-example.html.

DeleteHi Jason,

ReplyDeleteI got an error when I want to extract the mass matrix on the same way (it says that mass is not existing) do we need to do something more ?

Thank you

You first need create the *.full where the matrix is (WRFULL). The above example here would not have mass matrix as no density was previously defined for LINK1 elements.

DeleteOkay it works now, thanks again !

DeleteHi dear Jason

ReplyDeleteI've defined density and I tried to extract mass matrix but the mass and stiffness matrix both was looks exactly like each other. Please write the mass matrix code.

Thank you 💐

These commands should work:

Delete*SMAT, MatM, D, import, full, file.full, MASS

*PRINT, MatM, MatM, txt

Thank you so much ,That worked.

DeleteI have another question. I'm modeling something and after solving i extract stiffness and mass matrix and then i'm trying to model another thing but i can't extract the stiffness and mass matrix of the new model, when i run the commands of mass and stiffness matrix, ANSYS saves the previous model's mass and stiffness matrix for me!

what should i do?

Perhaps look at Multiframe restart (https://www.sharcnet.ca/Software/Ansys/16.2.3/en-us/help/ans_bas/Hlp_G_BAS3_12.html#BASmultrestmap52199). Inserting your script after the first and last FINISH command in example 5.1 yields different stiffness matrix file.

Deletehello sir,

ReplyDeleteThere is an error when i try to run the code, it says:

*SMA Command : Fails to open the file file.full.

*PRI Command : Matrix/Vector MATK cannot be found

*EXP Command : Matrix/Vector MATK cannot be found

It sounds like Ansys was not able to locate file.full. Make sure you have it in the working directory before *SMAT is issued.

Delete