WORKSHOP 4 Structure Subjected to Enforced Displacement at an incline презентация

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.

= 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

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.

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.

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

frame.
Select Coord 1 for the Analysis Coordinate Frame.
Click on Node 7
Click Apply.

Step 3. Finite Element: Modify /Node /Edit

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

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

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.

text input
Click on the button-Case Control Section.
Enter TEMP(INIT)=20
Click OK.

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

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.

$ 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.

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.

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