Shell Edge Contact

Chapter 49: Shell Edge Contact

49

Shell Edge Contact



Summary



Introduction



Modeling Details



Solution Procedure



Results



Modeling Tips



Pre- and Postprocess with SimXpert



Input File(s)



Video

994 995 995 1000

1001

1036

1003

1035

1004

994 MD Demonstration Problems CHAPTER 49

Summary Title

Chapter 49: Shell Edge Contact

Features

Case 1: In-plane glued edge deformable-deformable contact Case 2: General shell edge deformable-deformable contact

Geometry

Units: m, N, s

Units: in, lbf, s y' z'

y'

x'

x' shell edge contact

z' y 45o

10.0 m

z' shell edge contact x'

z

5 x 2 x 0.05

y'

x 10.0 m

Case 1: Modal Analysis of a Thick Rombic Plate

Material properties

Case 2: Diagonal Crushing of Square Tube

Case 1: E = 200GPa ,  = 0.3 ,  = 8000  kg  m3  Case 2: E = 2.1x10 11 psi ,  = 0.3

Analysis characteristics

Case 1: Modal analysis using in plane glued edge contact Case 2: Quasi-static analysis using general shell edge contact

Boundary conditions

• Case 1: Upper and lower half of plate are connected using glued edge contact Fixed conditions at all four edges In-plane displacements restrained at all nodes except those nodes at the edges of the glued contact line • Case 2: Edge-to-edge contact between two square tubes Clamped condition at bottom edge of lower tube

Applied loads

Case 2: Move top edge of top tube down two inches.

Element type

4-node shell elements

FE results

Displacement Contours Case 1: Mode 1 134.18 Hz

Seam

CHAPTER 49 995 Shell Edge Contact

Introduction The 3-D contact capability introduced in MD Nastran R2 supported a general node to surface contact in all translational degrees of freedom. The feature of shell edge to shell edge contact was added in the R3 release of MD Nastran. The following two cases are considered to demonstrate two different types of shell edge contact. Case 1:

Modal analysis of thick rhombic plate. This is a NAFEMS test case involving evaluation of natural frequencies of a fully clamped rhombic plate. The plate is divided into two equal parts in the vertical direction. These two parts are meshed with different mesh densities and then connected with in-plane glued edge contact.

Case 2:

Diagonal crushing of two square tubes. This model demonstrate the capability of general shell edge contact by crushing the lower square tube with the upper square tube as a result of the edge contact between the two tubes.

Modeling Details MD Nastran's solution sequences 103 and 400 are used to demonstrate the shell edge contact capability with the two test cases. The details of the finite element model, contact simulation, material, load, boundary conditions, and solution procedure for these two models are discussed below. Case 1: Two equal parts of rhombic plate are meshed with different mesh densities of 16 x 32 and 20 x 40 CQUAD4 elements. These two parts do not share any node at their common edge as they are connected using in-plane glued edge contact. The FE model used for the modal analysis (SOL 103) shown in Figure 49-1 and the case control section part of the input is given below: SUBCASE 1 METHOD = 1 BCONTACT = 1 SET 10 = 1,2,3,4,5,6 SET 20 = 137,182,213,280,327,593,600,639,703,744 SPC = 2 OMODE = 10 DISP(PLOT,PUNCH)=20 The modal analysis method to be used for extracting the eigenvalues is referenced by the METHOD option, and the associated contact table to be used is referenced by the BCONTACT option. The SPC option refers to the set of boundary conditions to be applied and the OMODE option identifies the list of modes to be extracted.

996 MD Demonstration Problems CHAPTER 49

Case 1

Case 2

bsurf-1

bsurf-1

bsurf-2

bsurf-2

Y Z

X

Y

X Z

Figure 49-1

FE Models used for Cases 1 and 2 of Shell Edge Contact

Case 2: The rectangular sides of each square tube are meshed using 5x10 CQUAD4 elements. The FE details for the SOL 400 analysis of Case 2 are given in Figure 49-1. The case control section part of the input for this model is given below: SUBCASE 1 STEP 1 ANALYSIS = NLSTATIC NLPARM = 1 BCONTACT = 1 SPC = 2 LOAD = 1 DISPLACEMENT(SORT1,REAL)=ALL SPCFORCES(SORT1,REAL)=ALL STRESS(SORT1,REAL,VONMISES,BILIN)=ALL BOUTPUT(SORT1,REAL)=ALL This section defines convergence controls via NLPARM, contact table and parameters via BCONTACT, applied displacements and loads via SPC and LOAD, and the displacements, stress, and contact results for the output file.

Material Modeling The isotropic, Hookean elastic material properties of the deformable body for Case 1 are defined in the SI (international) system using the following MAT1 option: MAT1

1

2.+11

.3

8000.

The MAT1 entry for Case 2 is given in the same system below: MAT1

1

2.1+11

.3

1.

CHAPTER 49 997 Shell Edge Contact

Element Modeling Besides the standard options to define the element connectivity and grid coordinate location, the bulk data section contains various options with special relevance to nonlinear analysis. For the SOL 400 analysis of Case 2, the nonlinear extensions to the lower-order shell element, CQUAD4, are activated by using the PSHLN1 property option in conjunction with the regular PSHELL property option in the manner shown below: PSHELL PSHLN1

1 1 C4

1 1 DCT

.05

1

1

L

For the modal analysis of Case 1, regular CQUAD4 elements are defined using the following PSHELL option. PSHELL

1

1

1.

1

1

Modeling Contact The BCPARA option used for the Case 2 model is given below. It defines the number of bodies in contact, together with the maximum number of contact entities (e.g. patches), nodes on the periphery of the contact surfaces and bias factor. The general shell edge contact option is enabled by activating the beam to beam contact flag BEAMB. BCPARA

0 BIAS

NBODIES 2 .95 BEAMB

MAXENT 1

400

MAXNOD

220

The definition of the contact bodies consists of the BCBODY Bulk Data Entry which defines the deformable body including the body ID, dimensionality, type of body, type of contact constraints and friction, etc. while the BSURF identifies the elements forming a part of the deformable body. The following BCBODY entries are used for cases 1 and 2. Figure 49-2 identifies the contact bodies used in both these models. BCBODY BSURF

Figure 49-2

1 1 8 16 …

3D 1 9 17

DEFORM 2 10 18

1 3 11 19

0 4 12 20

Contact Status Plot for Modal Analysis (Case 1)

5 13 21

6 14 22

7 15 23

998 MD Demonstration Problems CHAPTER 49

To identify the interaction between the contact bodies, the BCTABLE Bulk Data Option is used. BCTABLE with ID 0 is used to define the touching conditions at the start of the analysis. This is a mandatory entry required in SOL 400 for contact analysis and it is flagged in the case control section through the optional BCONTACT = 0 option. The BCTABLE with ID 1 is used to define the touching conditions for later increments in the analysis, and it is flagged using BCONTACT = 1 in the Case Control Section. A contact option, COPT, in BCTABLE allows more advanced control on how the contact bodies should interact with each other. COPT is defined using the formula COPT= =A+10*B+1000*C, where the terms A, B, and C are defined as follows: A: the outside of the solid elements in the body = 1:

the outside will be in the contact description (DEFAULT)

B (flexible bodies): the outside of the shell elements in the body = 1:

both top and bottom faces will be in the contact description, thickness offset will be included (DEFAULT)

= 2:

only bottom faces will be in the contact description, thickness offset will be included

= 3:

only bottom faces will be in the contact description, shell thickness will be ignored

= 4:

only top faces will be in the contact description, thickness offset will be included

= 5:

only top faces will be in the contact description, shell thickness will be ignored

= 6:

both top and bottom faces will be in the contact description, shell thickness will be ignored

Note if B = 6 for both bodies in a contact combination, then nodes that separate from a body, cannot come in contact again in the current step or in subsequent steps unless a different flag is chosen for one of the bodies. B (rigid bodies): the rigid surface = 1:

the rigid surface should be in the contact description (DEFAULT)

C (flexible bodies): the edges of the body = 1:

only the beam/bar edges are included in the contact description (DEFAULT)

= 10: only the free and hard shell edges are included in the contact description = 11: both the beam/bar edges and the free and hard shell edges are included in the contact description Note that C has no effect if beam-to-beam contact is not switched on (i.e., BEAMB is left as 0 on BCPARA). The following BCTABLE entries are used for the SOL 103 analysis of Case 1: BCTABLE

1 SLAVE

2 0 FBSH

0. 0 1.+20

1 0. 0 0.

0. 0.

0.

3 60

60

CHAPTER 49 999 Shell Edge Contact

It is important to note that the in-plane edge glued contact is activated by assigning value 60 for COPTS1 and COPTM1 in the 4th line of the BCTABLE option. The value 60 (B = 6) signifies that the edges are checked for contact without taking the shell thickness into account. Glued contact is defined by using a value of 3 for IGLUE in the 2nd line of the BCTABLE option. The value of IGLUE=3 allows moments to be transmitted across the contacting interface. JGLUE=0 in the 3rd field of the 3rd line ensures that glued nodes do not separate during the modal analysis. The contact status plot for Case 1 is presented in Figure 49-2. For the SOL 400 analysis of Case 2, the regular shell edge contact option is activated by assigning value of 10010 (B=1 and C=10) for COPTS1 and COPTM1 in the following BCTABLE entries: BCTABLE

BCTABLE

0 SLAVE

2 0 FBSH MASTERS 1 1 SLAVE 2 0 FBSH MASTERS 1

0. 0 1.+20

1 0. 0 0.

0. 0 1.+20

1 0. 0 0.

0.

0.

0. 0.

0 10010

0.

0.

10010

0 10010

10010

B = 1 in the definition of the COPT flags indicates that the thickness and both faces are considered for contact and C = 10 indicates that the shell edges are included in the contact description.

Loading and Boundary Conditions For the SOL 103 analysis (Case 1), the boundary conditions are applied through the following SPC cards. No additional loads are applied for this analysis. SPCADD SPC1 SPC1 … SPC1 SPC1

2 1 1

1 126 126

3 1 25

THRU THRU

23 44

3 3

123456 123456

1 44

THRU 65

23 86

107

128

149

For the SOL 400 analysis (Case 2), the loading and boundary conditions are applied with the following SPCD and SPC cards. SPCADD FORCE SPCD SPCD … SPC1 SPC1 SPC1

2 1 1 1

1 1 1 3

3

1 1 3

123456 123456 123456

36 391 1

3 3

0. 2. 2. THRU THRU

.57735 2 4

.57735 3 3

.57735 2. 2.

400 20

The loading and boundary conditions applied for Cases 1 and 2 are presented in Figure 49-3. For Case 1, the displacements u x = u y =  z = 0 for all nodes and u z =  x =  y = 0 along all edges as shown in Figure 49-3

1000 MD Demonstration Problems CHAPTER 49

except that the in-plane translation boundary condition for are not applied at the interface of the contact bodies so that they do not conflict with the in-plane glued edge contact constraints.

Case 1

Case 2

Figure 49-3

Loading and Boundary Conditions for Cases 1 and 2

Solution Procedure The modal analysis SOL 103 procedure for Case 1 is defined with the following EIGRL entry: EIGRL

1

100.

500.

6

0

MASS

The six frequencies in the range 100 to 600 are requested through the above option. The SOL 4 00 nonlinear procedure for Case 2 is defined through the following NLPARM entry: NLPARM

1

10 0.1

PFNT

1 0

PV

NO

0

0 The number of increments is provided in the 3rd field of the 1st line of NLPARM option. PFNT represents Pure Full Newton Raphson technique wherein the stiffness is reformed at every iteration. The value of KSTEP=1 along with PFNT option indicates that the stiffness matrix will not be updated between the convergence of a load increment and the start of the next load increment. PV indicates that the maximum vector component of the residuals will be checked for convergence. NO indicates that intermediate output will not be produced after every increment. The second line of NLPARM indicates that a tolerance of 0.1 will be used for convergence checking. The nonlinear procedure also deactivates Quasi-Newton, line search and cutbacks by assigning the value of 0 for MAXQN, MAXLS, and MAXBIS.

CHAPTER 49 1001 Shell Edge Contact

Results Frequencies of 6 modes extracted from the modal analysis are indicated in the Table 49-1. It clearly shows that the in-plane glued edge contact can be successfully used to assemble parts with different mesh densities, since the predictions are within a 2% error. The mode shapes of the six modes for rhombic plate are presented in Figure 49-4. Table 49-1

Comparison of Frequencies with NAFEMS Results

Mode Number

SOL 103 Frequency Hz

NAFEMS Frequency Hz

%Error

1

134.18

133.95

0.17

2

204.37

201.41

1.47

3

270.59

265.81

1.80

4

284.56

282.74

0.64

5

341.13

334.45

2.0

6

385.79

NA

-

Figure 49-4

Mode 1: 134.18 Hz

Mode 2: 204.37 Hz

Mode 3: 270.59 Hz

Mode 4: 284.56 Hz

Mode 5: 341.13 Hz

Mode 6: 385.79 Hz

Mode Shapes of Thick Rhombic Plate

1002 MD Demonstration Problems CHAPTER 49

Figures 49-5 and 49-6 demonstrate that the shell edge contact is properly detected as the top tube crushes the lower tube. Contact Status

50 % Load

Figure 49-5

100 % Load

Contact Status Plots for Square Tubes with Shell Edge Contact Z-Displacement

50 % Load

Figure 49-6

100 % Load

Original and Deformed Shapes of Square Tubes with Shell Edge Contact

CHAPTER 49 1003 Shell Edge Contact

Modeling Tips The most important aspect in the shell edge contact analysis is the COPT options introduced in BCTABLE. This gives more flexibility for users to define the interaction between different contact bodies (solid or shell or beam elements). Readers can observe the changes in results for the two cases presented in this chapter by removing the COPT options in BCTABLE. It is also possible to define the COPT options in the BCPARA and BCBODY options. The options ITOPBM, ITOPSH, and ITOPSL in the BCPARA option and COPTB in the BCBODY option can be used to define the same COPT option in cases where BCTABLE is not used in the model with BCONTACT=ALLBODY option. This is recommended as an exercise for the readers. It is important to remember that the general shell edge contact capability is activated by setting the beam to beam contact flag option BEAMB to 1 in BCPARA entry.

1004 MD Demonstration Problems CHAPTER 49

Pre- and Postprocess with SimXpert This example will take you through Case 2 of the Shell Edge Contact Cases. The required input file can be downloaded by clicking the nug_49b.dat link in the Input File(s) section of this document.

Specify the Model Units a. Tools: Options b. Select Units Manager c. For Basic Units, specify the model units Length = mm; Mass = kg; Time = s; Temperature = kelvin, Force = N d. Click OK

a

b

c

a d

CHAPTER 49 1005 Shell Edge Contact

Import FE Mesh a. File b. Select Import c. Select Nastran d. Select nug49_mesh.bdf e. Click Open

a

b

c

d

e

1006 MD Demonstration Problems CHAPTER 49

Set Model View a. View b. Select Model Views c. Select Front d. Select Fill

a d

b

c

CHAPTER 49 1007 Shell Edge Contact

Define Material a. Materials and Properties tab b. Material, select Isotropic c. Young’s Modulus: enter 2.1e11 d. Poisson’s Ratio: enter 0.3 e. Click OK

a b

c d

e

1008 MD Demonstration Problems CHAPTER 49

Define Property Data a. Materials and Properties tab b. 2D Properties, select Shell c. Entities: select PSHELL_nug49_mesh.bdf d. Material: select Iso_1 e. Part thickness: enter 0.05 f. Click Advanced

a b

c d e

f

c d

CHAPTER 49 1009 Shell Edge Contact

Define Property Data (continued) a. Click Non Linear b. Membrane material, select Iso_1 c. Bending material: select Iso_1 d. Analysis type: select IS e. Corner elements keyword: select C4 f. Element structural behaviour: select DCT g. Integration scheme: select L h. Click OK

b

a b c d e

g

f

h

c

1010 MD Demonstration Problems CHAPTER 49

Define Contact Body for Lower Part a. LBCs tab b. Contact, select Deformable Body c. Name: enter body_lower d. Type: select Deformable Surface e. Pick Entities: select 200 Elements f. FEM filters: select Pick Elements g. Select elements from lower part of shell h. Click OK

a b

c d e

f g h

CHAPTER 49 1011 Shell Edge Contact

Define Contact Body for Upper Part a. LBCs tab b. Contact, select Deformable Body c. Name: enter body_upper d. Type: select Deformable Surface e. Pick Entities: select 200 Elements f. FEM filters: select Pick Elements g. Select elements from upper part of shell h. Click OK

a b

g c d e

f h

1012 MD Demonstration Problems CHAPTER 49

Define Contact Table a. LBCs tab b. Contact, select Table c. Click Deactivate All d. Touching Condition for body 1: set to 2 e. Distance Tolerance: enter 0 f. Individual Contact Detection: select Double Sided g. Individual Slave Option Flag: select 100010 h. Individual Master Option Flag: select 10010 i. Click OK

a

b

c d

e

f

g h i

CHAPTER 49 1013 Shell Edge Contact

Define Boundary Conditions a. LBCs tab b. Constraints, select Fixed c. Name: enter fix-z d. Entities: select nodes at the top edge of body_upper e. Click OK

a b

d

c d

e

1014 MD Demonstration Problems CHAPTER 49

Define Boundary Conditions (continued) a. LBCs tab b. Constraints, select General c. Name: enter disp-z d. Entities: select nodes at the top edge of body_upper e. Tz: select 2.0 f. Click OK

a b

c

d

e

f

d

CHAPTER 49 1015 Shell Edge Contact

Analysis Setup a. Model Browser: right click FileSet (nug49_mesh) b. Select Create new Nastran job c. Name: enter ch49b d. Solution Type: select SOL400 e. Solver Input File: select ch49b.bdf f. Uncheck Create Default Layout g. Click OK

a b c

d e

f

g

1016 MD Demonstration Problems CHAPTER 49

Analysis Setup (continued) a. Model Browser: nug49_mesh.bdf, ch49b, right click Load Case b. Select Create Global Loadcase c. Click OK

a b

c

CHAPTER 49 1017 Shell Edge Contact

Analysis Setup (continued) a. Model Browser: nug49_mesh.bdf, ch49b, right click Loads/Boundaries b. Select Select Contact Table c. Selected BCT Table, select BCTABLE_1 d. Click OK e. Model Browser: nug49_mesh.bdf, ch49b, right click Load Case e. Select Create Loadcase g. Name (Title): enter subcase-1 h. Click OK

a

b

c

d

e

f g

h

1018 MD Demonstration Problems CHAPTER 49

Analysis Setup (continued) a. Model Browser: Load Cases, subcase-1, double click Load Case Control b. Select Subcase Nonlinear Static Parameters c. Stiffness Update Method: select PFNT d. Uncheck Use Default Tolerance Setting e. Check Load Error, for Load Tolerance: enter 0.01 e. Check Vector Component Method g. Intermediate Output Control: select Yes h. Click Apply i. Click Close

a

b c

d

e e

f g

h i

CHAPTER 49 1019 Shell Edge Contact

Analysis Setup (continued) a. Model Browser: double click Load Case Control b. Select Stepping Procedure Parameters c. Number of Steps: enter 10 d. Click Apply e. Click Close

a

b c

d e

1020 MD Demonstration Problems CHAPTER 49

Analysis Setup (continued) a. Model Browser, subcase-1, right click Load/Boundaries b. Select Select Lbcs c. From Model Browser with control key and mouse, select fix-z and disp-z d. Click OK

a b c c

d

CHAPTER 49 1021 Shell Edge Contact

Analysis Setup (continued) a. Model Browser, subcase-1, right click Load/Boundaries b. Select Contact Table c. Selected BCT Table, select BCTABLE_1 d. Click OK

a

b c

d c

1022 MD Demonstration Problems CHAPTER 49

Analysis Setup (continued) a. Model Browser, subcase-1, right click Output Request b. Select Nodal Output Requests c. Select Create Displacement Output Request d. Check Suppress Print Click OK

c d

a b e

CHAPTER 49 1023 Shell Edge Contact

Analysis Setup (continued) a. Model Browser, subcase-1, right click Output Request b. Select Nodal Output Requests c. Select Create Contact Output Request d. Check Suppress Print Click OK

c d

a b

e

1024 MD Demonstration Problems CHAPTER 49

Analysis Setup (continued) a. Model Browser, subcase-1, right click Output Request b. Select Elemental Output Requests c. Select Create Nonlinear Stress Output Request d. Check Suppress Print e. Click OK

a b

c d

e

CHAPTER 49 1025 Shell Edge Contact

Analysis Setup (continued) a. Model Browser, ch49b, double click Solver Control b. Contact Control Parameters, select Contact Detection Parameters c. Distance Tolerance, enter 0 d. Bias on Distance Tolerance: enter 0.9 e. Click Activate 3D Beam-Beam Contact f. Click Apply g. Click Close

a

c d e

b

f g

1026 MD Demonstration Problems CHAPTER 49

Analysis Setup (continued) a. Model Browser, ch49b, double click Solver Control b.Select Output File Properties c. Nastran DB Options, select Master/DBALL d. Binary Output: select OP2 e. Click Apply Click Close (not shown)

a

b

c

d

e

CHAPTER 49 1027 Shell Edge Contact

Analysis a. File, click Save b.Model Browser, right click ch49b c. Select Run d. Click Save (after completion of job) e. File, click New

a b

c

e

d

1028 MD Demonstration Problems CHAPTER 49

Postprocessing a. File, click Attach Results b.File path: select MASTER c. Attach Options: select Both d. Click OK

a b c

d

CHAPTER 49 1029 Shell Edge Contact

Postprocessing (continued) a. Results tab b.Results: select Deformation c. Deformed display scaling: select True d. Click Plot Data tab e. Plot attribute, Plot type, Deformation f. Result Cases, select last increment g. Result Type, select Displacements, Translational h. Click Update

a b

c

d h e

g

f

1030 MD Demonstration Problems CHAPTER 49

Postprocessing (continued) a. State plot property editor b.Check Animate c. Result Cases, select SC1_Step1 d. Result Type, select Displacements, Translational e. Click Update

a

e

d b

c

CHAPTER 49 1031 Shell Edge Contact

Postprocessing (continued) a. Click Pause icon

a

1032 MD Demonstration Problems CHAPTER 49

Postprocessing (continued) a. Results tab b.Results: select Fringe c. Check Animate d. Result Cases, select SC1_Step1 e. Result Type, select contactforce,Normal f. Click Fringe tab g. Element edge display, Display, select Element edges h. Click Label attributes tab i. Select appropriate color for labels j. Click Update

a b

c

d

f

g

h i

j

e

CHAPTER 49 1033 Shell Edge Contact

Postprocessing (continued)

1034 MD Demonstration Problems CHAPTER 49

Postprocessing (continued) a. Click Pause icon b.Click Plot Data tab c. Result Type, select Nonlinear Stresses d. Derivation, select X Component e. Click Update

a

b e

c d

CHAPTER 49 1035 Shell Edge Contact

Postprocessing (continued)

Input File(s) File

Description

nug_49a.dat

MD Nastran input for modal analysis of rhombic plate (Case 1)

nug_49b.dat

MD Nastran input for diagonal crushing of square tubes (Case 2)

1036 MD Demonstration Problems CHAPTER 49

Video Click on the image or caption below to view a streaming video of this problem; it lasts approximately nine minutes and explains how the steps are performed.

Contact Status

50 % Load

Figure 49-7

Video of the Above Steps

100 % Load