Reaction Forces from enforced displacments

[Fnsman810]

Hello,

We are trying to determine the force required to create an enforced displacement. We are deflecting a part 2 mm using Design Simulation, and I assumed I could use the magnitude of the Reaction Force as the force required. When I rerun the simulation using that force, I am not getting the same displacement.

Is there another way to determine the force required to create the enforced displacement? Am I misinterpreting the reaction force information?

Thanks.

 

[BlasMolero]

Hello!,
You need to use RBE2 elements in order to control the "exact" behaviour of the model. The problem is that NX Design Simulation do not support 1-D Rigid RBE2 elements.
In summary, if you apply a force load the reaction should be exactly the same value but reversed, then if you prescribe the resultant displacements as enforced loading you will get the same reaction.
But this should be done carefully in order the get "exactly" results.

You need to use a SPIDER type connection (not available under Design Simulation), where you connect a single node (the core node) to multiple nodes (leg nodes) with a rigid or constraint element named RBE2 using a point-to-face connection. Using this mechanism you can apply a force to the core node of the RBE2 and read the resultant displacement in that node. Next you CLONE the study, delete the force load and prescribe the previous resultant displacement as enforced-displacement, then ypu will se that REACTION FORCE will be exactly equal in both analysis.

In RBE2 elements the active degrees of freedom of the single core node (independent) enforce the active degrees of freedom of the leg nodes (dependent). Therefore, the active degrees of freedom of all nodes included in an RBE2 element are considered rigidly connected.

Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[mechanik1208]

Hello,

I have similar problem with a 3D model in NX 8.0.
I have used tetrahedral elements for a plastic isotropic assigned material. The enforced displacement doesn't give the
exact reaction force and in another simulation the load constraint doesn't match the applied force result.

My question is is it possible to apply RBE2 elements to a 3D model in NX 8.0. All i did was to select the edges(1D application) of my
3D model and assigned RBE2 elements. But as expected, NX solver shows error for over lapping constraints.

Is there any other way to do it in NX ?

Regards,
mechanik1208

 

[BlasMolero]

Dear Mechanik,
RBE2 elements is THE BEST method to prescribe enforced displacement, not doubt at all, is simply an elegant, but you must be aware of NOT TO PRESCRIBE ANY CONSTRAINT to DEPENDENT nodes of RBE2 legs, in this case NX NASTRAN will give you error as a double dependency exist, is impossible to obey to two masters at the same time!!. Then when prescribing constraints make sure yuo EXCLUDE the nodes belonging to dependent nodes of RBE2 elements, OK?.
Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[mechanik1208]

Hello,

Thanks for the quick reply.
I would like to address the following things.
1) I tried to generalize my problem in nx. So i took a simple cantilever beam and applied enforced displacement. The reaction forces do not match the deflection force(which i applied in the next simulation
to verify the displacement). Hence, the same problem exists with any model.
2) I discussed this issue with my senior colleagues and they want to know why do we need to apply RBE2 element in the first place ? They want to verify the process of enforced displacement again without RBE2 which i doubt would yield success.

3) Coming to my problem, taking a simple cantilever example. I would like to know how do you correctly apply the RBE2. I am mentioning the steps, please correct me if i am wrong.
- first you mesh the model in fem file.
- now select the edge on which you want apply the load and assign RBE2 elements to it. Here comes my doubt, is there another place where you assign the RBE2 element ? If i apply it on the edge, then in the simulation file when i apply enforced displacement on the same edge nx solver shows error. As you said there cant be two masters.
So I want to know where do you apply the RBE2 element in a simple cantilever beam example.
thank you,
Regards,
mechanik1208

 

[BlasMolero]

Dear Mechanik,
Well, is your word, I don't know the way you do things exactly, in the comparison is the devil!.
Play with simply models, use a simply cantilever beam meshed with 1-D CBEAM elements, in this case not need to use at all any RBE2 element.
Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[mechanik1208]

Hello,

I would appreciate a constructive advice rather than sarcasm.
Please forgive my ignorance, but i hope you understood the problem that i was trying to state.
Even with a simple cantilever model, first you give enforced displacement, then calculate strain and reaction force.
Now, if this reaction force is treated as an applied load in the next simulation, then the displacement is not the same as the first case.

Could you give me the reason as to why the reaction force is not equal to the applied load which would have caused the same displacement ?
Now as this problem exists even in a simple cantilever, what is the solution ? as you say RBE2 elements cannot be applied to this simple model.

regards,
mechanik

 

[BlasMolero]

Dear Mechanik,
This is a very basic task, I suggest to contact your NX VAR or RESELLER to get CAE training in NX AdvSim & NX NASTRAN, this is critical.
Here you are a simply steel cantilever beam of 10x5 mm cross section and length 100 mm.

CANTILEVER1 (model left)
================
• One end fully constrained and at the other end a prescribed displacement of TZ=1 mm. Model solved and you get maximum beam stress = 154.2 MPa, and maximum displacement = 1mm.
• If I look to results I see reaction force at fixed node TZ=6.425229E+01. This should be the force loading to apply to the next model.

                               [b]F O R C E S   O F   S I N G L E - P O I N T   C O N S T R A I N T[/b]
 
      POINT ID.   TYPE          T1             T2             T3             R1             R2             R3
             1      G      0.0            0.0           -6.425229E+01   0.0            6.425229E+03   0.0
            11      G      0.0            0.0            6.425229E+01   0.0            0.0            0.0

• You can import the nastran deck in your NX AdvSim and rerun the model as well, simply copy & paste the next input:

INIT MASTER(S)
NASTRAN SYSTEM(442)=-1,PARALLEL=8,SYSTEM(319)=1
ID cantilever1,Femap
SOL SESTATIC
TIME 10000
CEND
  TITLE = NX NASTRAN (SOL101)
  ECHO = NONE
  DISPLACEMENT(PRINT) = ALL
  SPCFORCE(PRINT) = ALL
  OLOAD(PRINT) = ALL
  FORCE(PRINT,CORNER) = ALL
  STRESS(PRINT,CORNER) = ALL
  SPC = 1
  LOAD = 1
BEGIN BULK
$ ***************************************************************************
$   Written by : Femap with NX Nastran
$   Version    : 11.1.0
$   Translator : NX Nastran
$   From Model : D:\MODELOS\TEST\cantilever1.modfem
$   Date       : Wed Nov 13 22:37:31 2013
$   Output To  : D:\SCRATCH
$ ***************************************************************************
$
PARAM,OGEOM,NO
PARAM,AUTOSPC,YES
PARAM,K6ROT,100.
PARAM,GRDPNT,0
CORD2C         1       0      0.      0.      0.      0.      0.      1.+FEMAPC1
+FEMAPC1      1.      0.      1.        
CORD2S         2       0      0.      0.      0.      0.      0.      1.+FEMAPC2
+FEMAPC2      1.      0.      1.        
$ Femap with NX Nastran Load Set 1 : DESPLAZAMIENTO_PRESCRITO
SPCD           1      11       3      1.
$ Femap with NX Nastran Constraint Set 1 : RESTRICCIONES
SPC1           1  123456       1
SPC1           1       3      11
$ Femap with NX Nastran Property 1 : Bar_10x5mm
$ Femap with NX Nastran PropShape 1 : 1,0,10.,5.,0.,0.,0.,0.
$ Femap with NX Nastran PropOrient 1 : 1,0,0.,1.,2.,3.,4.,-1.,0.,0.
PBEAM          1       1     50.104.1667416.6667      0. 286.212      0.+       
+           -2.5     -5.     2.5     -5.     2.5      5.    -2.5      5.+       
+           YESA      1.                                                +       
+       .8507012.8499302                                                        
$ Femap with NX Nastran Material 1 : Acero (MPa)
MAT1           1 206000.              .3  7.85-9 1.728-5      0.        +       
+           235.    340.        
MAT4           1    .014 434000.  7.85-9                        
GRID           1       0      0.      0.      0.       0
GRID           2       0     10.      0.      0.       0
GRID           3       0     20.      0.      0.       0
GRID           4       0     30.      0.      0.       0
GRID           5       0     40.      0.      0.       0
GRID           6       0     50.      0.      0.       0
GRID           7       0     60.      0.      0.       0
GRID           8       0     70.      0.      0.       0
GRID           9       0     80.      0.      0.       0
GRID          10       0     90.      0.      0.       0
GRID          11       0    100.      0.      0.       0
CBEAM          1       1       1       2      0.      0.      1.
CBEAM          2       1       2       3      0.      0.      1.
CBEAM          3       1       3       4      0.      0.      1.
CBEAM          4       1       4       5      0.      0.      1.
CBEAM          5       1       5       6      0.      0.      1.
CBEAM          6       1       6       7      0.      0.      1.
CBEAM          7       1       7       8      0.      0.      1.
CBEAM          8       1       8       9      0.      0.      1.
CBEAM          9       1       9      10      0.      0.      1.
CBEAM         10       1      10      11      0.      0.      1.
ENDDATA c640e79c

CANTILEVER2 (model right)
=================
• One end fully constrained and the other an applied load FZ==6.425229E+01 N. Model solved and you get maximum beam stress = 154.2 MPa and maximum displacement = 1mm.
• Here you are the nastran input deck, simply import in NX AdvSim and you are done!:

INIT MASTER(S)
NASTRAN SYSTEM(442)=-1,PARALLEL=8,SYSTEM(319)=1
ID cantilever2,Femap
SOL SESTATIC
TIME 10000
CEND
  TITLE = NX NASTRAN (SOL101)
  ECHO = NONE
  DISPLACEMENT(PRINT) = ALL
  SPCFORCE(PRINT) = ALL
  OLOAD(PRINT) = ALL
  FORCE(PRINT,CORNER) = ALL
  STRESS(PRINT,CORNER) = ALL
  SPC = 1
  LOAD = 1
BEGIN BULK
$ ***************************************************************************
$   Written by : Femap with NX Nastran
$   Version    : 11.1.0
$   Translator : NX Nastran
$   From Model : D:\MODELOS\TEST\cantilever2.modfem
$   Date       : Wed Nov 13 22:44:49 2013
$   Output To  : D:\SCRATCH
$ ***************************************************************************
$
PARAM,OGEOM,NO
PARAM,AUTOSPC,YES
PARAM,K6ROT,100.
PARAM,GRDPNT,0
CORD2C         1       0      0.      0.      0.      0.      0.      1.+FEMAPC1
+FEMAPC1      1.      0.      1.        
CORD2S         2       0      0.      0.      0.      0.      0.      1.+FEMAPC2
+FEMAPC2      1.      0.      1.        
$ Femap with NX Nastran Load Set 1 : CARGA_APLICADA
FORCE          1      11       0      1.      0.      0.64.25229
$ Femap with NX Nastran Constraint Set 1 : RESTRICCIONES
SPC1           1  123456       1
$ Femap with NX Nastran Property 1 : Bar_10x5mm
$ Femap with NX Nastran PropShape 1 : 1,0,10.,5.,0.,0.,0.,0.
$ Femap with NX Nastran PropOrient 1 : 1,0,0.,1.,2.,3.,4.,-1.,0.,0.
PBEAM          1       1     50.104.1667416.6667      0. 286.212      0.+       
+           -2.5     -5.     2.5     -5.     2.5      5.    -2.5      5.+       
+           YESA      1.                                                +       
+       .8507012.8499302                                                        
$ Femap with NX Nastran Material 1 : Acero (MPa)
MAT1           1 206000.              .3  7.85-9 1.728-5      0.        +       
+           235.    340.        
MAT4           1    .014 434000.  7.85-9                        
GRID           1       0      0.      0.      0.       0
GRID           2       0     10.      0.      0.       0
GRID           3       0     20.      0.      0.       0
GRID           4       0     30.      0.      0.       0
GRID           5       0     40.      0.      0.       0
GRID           6       0     50.      0.      0.       0
GRID           7       0     60.      0.      0.       0
GRID           8       0     70.      0.      0.       0
GRID           9       0     80.      0.      0.       0
GRID          10       0     90.      0.      0.       0
GRID          11       0    100.      0.      0.       0
CBEAM          1       1       1       2      0.      0.      1.
CBEAM          2       1       2       3      0.      0.      1.
CBEAM          3       1       3       4      0.      0.      1.
CBEAM          4       1       4       5      0.      0.      1.
CBEAM          5       1       5       6      0.      0.      1.
CBEAM          6       1       6       7      0.      0.      1.
CBEAM          7       1       7       8      0.      0.      1.
CBEAM          8       1       8       9      0.      0.      1.
CBEAM          9       1       9      10      0.      0.      1.
CBEAM         10       1      10      11      0.      0.      1.
ENDDATA bf6f80d9

Best regards,
Blas.



~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[mechanik1208]

Hello,

Thank you for the explanation.
Its been very useful.

Regards,
mechanik