WORKSHOP 4 Structure Subjected to Enforced Displacement at an incline


The Presentation inside:

Slide 0

WORKSHOP 4 Structure Subjected to Enforced Displacement at an incline


Slide 1


Slide 2

Workshop 4 - Coordinate Systems and Constraints Using the truss model from Workshop 3, change the constraints and add a fourth loading condition. The new constraints will be a “roller” constraint along a 45 degree surface at the right edge (GRID point 7) In the additional loading condition: Apply a displacement of .05 units normal to the sloped surface Apply no other loads for this loading condition In order to do this, we will need to define a “displacement” coordinate system (CORD2R 100) for GRID 7 CORD2R,100,,576.,0.,0.,576.,0.,1. ,577.,1.,0.


Slide 3

Model for Workshop 4


Slide 4

New and Modified Case Control and Bulk Data for Workshop 4 TITLE = GARAGE ROOF FRAME SUBTITLE = WOOD AND STEEL MEMBERS DISPLACEMENT = ALL SPCFORCES = ALL STRESS = ALL SPC = 10 TEMP(INIT) = 20 SUBCASE 1 SUBTITLE=TRUSS_LBCS LOAD = 1 SUBCASE 20 SUBTITLE = THERMAL LOAD TEMP(LOAD) = 26 SUBCASE 30 SUBTITLE = GRAVITY LOAD LOAD = 30 SUBCASE 40 SUBTITLE = SUPPORT SETTLING LOAD = 40 BEGIN BULK CORD2R,100,,576.,0.,0.,576.,0.,1. ,577.,1.,0. SPCD,40,7,2,-.05 $ modified GRID 7 - displacement coordinate system GRID 7 576.0 0.0 0.0 100 345


Slide 5

Suggested Exercise Steps: Copy previous PATRAN workshop db file:w3.db to another name called w4.db Open the PATRAN database and bring in the w4.db Create a new coordinate system, and let GRID 7 uses this coordinate system as for the analysis frame. Create a new loadcase in PATRAN, (fourth loadcase) is called enforced_disp ,copy all the boundary conditions from the first loadcase to enforced_disp except the force loading. Create enforced displacement load in the new loadcase Submit the model to MSC.Nastran for analysis. Post-Process results using MSC.Patran.


Slide 6

Step 1. Load Case: Create /Load Case Name: enforced_disp Create a new load case: enforced_disp Type in enforced_disp for the Loadcase name. Click on the Assign/Prioritize Load/BCs button to bring up the menu on the far right. Click on the boundary conditions from the top left corner Select clamp, dof456, and rightside. Click OK to return to the main material menu. Click Apply.


Slide 7

Create a new coordinate system Create / Coord/ 3Point. Enter [576 0 0] for the Origin Enter [576 0 1] for the point on Axis 3. Enter [577 1 0] for Point on Plane 1-3 Click Apply. Step 2. Create Coord: Create/Coord/3Point


Slide 8

Modified the grid to use new analysis coordinate frame. Select Coord 1 for the Analysis Coordinate Frame. Click on Node 7 Click Apply. Step 3. Finite Element: Modify /Node /Edit


Slide 9

Create the enforced displacement loading Enter spcd as the new set name. Click Input Data, ENTER < , -0.05 ,> for the translations Put your cursor inside the Analysis Coordinate Frame box, and select the Coord 1 from the screen.Click OK to close the form Click on Select Application region and Changed the selection filter to FEM select Node 7 Click Add Click OK Click Apply. Step 4. Loads/BCs: Create /Displacement /Nodal


Slide 10

Step 4A: Plot of enforced displacement loading on grid 7


Slide 11

Modified the rightside boundary conditions for the new coord 1 Click rightside as the new set name. Click Modify Data, Changed the Analysis Coordinate Frame to Coord 1 Click OK to close the form Click on application region and select Node 7 Click Add Click OK Click Apply. Step 5. Loads/BCs: Modify/Displacement /Nodal


Slide 12

Step 5A: Plot of enforced displacement loading on grid 7


Slide 13

Step 5. Analysis: Analyze/ Entire Model/Analysis Deck Submit the model for analysis. Analyze / Entire Model / Analysis Deck. We will have to modified the existing test deck Click on the Solution Type. Select LINEAR STATIC as the Solution Type. Click OK. Click Direct Text input.


Slide 14

Step 6. Direct Text Input – Case Control Section Direct text input Click on the button-Case Control Section. Enter TEMP(INIT)=20 Click OK.


Slide 15

Step 7. Direct Text Input – Bulk Data Section Direct text input Click on Direct Text Input Click the button-Bulk Data Section. Enter TEMPD,20,70.0 Click OK. Click on the Subcase Select


Slide 16

Step 8. Analysis: Subcase Select Be sure the click the subcases in the following order Click On the Default from the top menu first. Followed by selecting thermal load, gravity load, and enforced_disp. Click OK. Click Apply.


Slide 17

Step 9. : Modified the existing analysis test deck $ Existing translations with PATRAN version 2001 $CASE CONTROL section SUBCASE 4 $ Subcase name : enforced_disp SUBTITLE=enforced_disp SPC = 2 LOAD = 7 DISPLACEMENT(SORT1,REAL)=ALL SPCFORCES(SORT1,REAL)=ALL STRESS(SORT1,REAL,VONMISES,BILIN)=ALL$ BEGIN BULK Loads for Load Case : enforced_disp SPCADD 2 18 19 20 17 Currently there is an translational error in PATRAN version 2001 writing out duplicate SPCADD bulk data entries.In order to correct this , the user needs to modified the bulk data cards as followed. Changed the SPC ID from 2 to 3 in the subcase 4 in the case control Changed the second SPCADD in the bulk data entries to SPCADD,3,18,19,20,17 Use notepad on your PC to open the translated test deck called:w4.bdf After editing the files then saved the filename as w4_m.dat. you can submit NASTRAN outside the PATRAN.


Slide 18

Step 10. Analysis: Attach XDB/ Result Entities/ Local Attach the XDB result file. Attach XDB / Result Entities / Local. Click on Select Result File. Select the file called w4_m.xdb Click OK. Click Apply.


Slide 19

Step 11. Results: Create/Quick Plot Create a Quick Plot of the results. Create / Quick Plot. Select SC4 result case. Select Displacement, Translational for the Deformation Result. Click Apply.


×

HTML:





Ссылка: