CAE notes Ex.2.3

Menu: 
	File, Save as, New directory [name of new directory], Select new directory, [name of file], OK
Module: Part, 
	Menu: Part, Create, Name[Part-1], 2D, Deformable, Shell, Approx size [200], Cont
	Menu: Add, Point, 
		[0,0]	# in the input window below the WS, then [Enter]
		[-20,0]
		[-40,0]
		[0,20]
		[0,40]
		[20,20]
		[20,40]
		F6    !to visualize
	Menu: Add, Arc, Center/Endpoints,
		# pick center point (see Fig. 2.7)
		# pick point left of center point
		# pick point above of center point, the arc is done
		# again pick center point (see Fig. 2.7)
		# pick point left-most of center point
		# pick point above-most of center point, the outer arc is done
		X	# to finalize the Add feature (do not click Done)
	Menu: Add, Lines, Connected	
		# pick two nodes to close bottom left of Fig. 2.7
		X   # to finalize the Line drawing
	Menu: Add, Lines, Connected	
		# pick 4 nodes in sequence to close rectangle at top right
		X   # to finalize the Line drawing
	Done    # to create the part

Module: Property
    Menu: Material, Create, 
		Name [Material-1], Mechanical, Elasticity, Elastic, 
		Type, Isotropic [195000, 0.3], OK
    Menu: Material, Create, 
		Name [Material-2], Mechanical, Elasticity, Elastic, 
		Type, Isotropic [210000, 0.3], OK

    Menu: Section, Create,
	# parameters that result from analytical integration are given in section
		# tricky: 	plane stress/strain is considered solid even though 
		#				pstres needs a thickness
		#				pstran does not
		#			shells are not solids, they need a thickness
		#			beams are not solids, they need area and moments of inertia
		Name [Section-1], Solid, Homo, Cont	
		Material [Material-1], 
		Plane stress/strain thickness [4.0]

	Menu: Assign, Section	# pick all (click on part), Done
		OK

Module: Assembly
	# if more than one part exist, assembly is obvious
	# for one part assemblies it is sort of trivial
    Menu: Instance, Create,
		Independent, OK

Module: Step
	# every analysis has a Initial step and at least one additional step
	# load cannot go on the Initial step (Abaqus will complain if you try)
    Menu: Step, Create, 
		Name [Step-1], General, Static/General, Cont
		OK
    
Module: Load
    Menu: Load, Create, 
		Name [load-1], Mechanical, Pressure, Cont
    # pick the vertical edge on the right, Done
		Magnitude [-9.5], OK
    Menu: BC, Create, 
		Name [BC-1], Step [Initial], Mechanical, Displacement/Rot, Cont
    # pick the horiz edge on bottom, Done
	#checkmark	U1, U2, UR3, OK
    Step: Step-1 	# to see the load and BC together
	
Module: Mesh
	Menu: Seed, Instance
		Approx global size [5.0], Apply, OK
    Menu: Mesh, Controls, Quad, Structured, Accept, OK
    Menu: Mesh, Element type, Standard, Linear, Plane stress, OK
    Menu: Mesh, Instance, Yes
    
Module: Job
    Menu: Job, Manager,
		Create, Name [Job-1], Model, Model-1, Cont, OK
		OK
		Data check, OK	# watch the execution window bellow the WS
		Submit, OK	# watch the execution window bellow the WS
		Results
    
Module: Visualization
	Menu: Plot, Contours, On Deformed Shape
	Menu: File, Save
	Menu: File, Exit