Optimizing the Crane Hook Model (Tosca Structure.gui)

This example shows a more general optimization setup using sensitivity based algorithms for shape optimization. Thus, the volume can be minimized considering as well stress and frequency constraints.

  1. Load the input files with the FEM_INPUT command.

  2. Define the Design Area (DV_SHAPE): 

    DV_SHAPE  
	ID_NAME	= MY_DV_SHAPE  
	ND_GROUP	= design_nodes
END_

    Note: If you are using MSC Nastran®, the group is defined as set 1 of the file cranehook_groups.bdf and can be loaded into Tosca Structure.guiin the command GROUP_DEF.

  3. Define the elements for mesh smoothing (MESH_SMOOTH): 

    MESH_SMOOTH  
	ID_NAME        = MY_MESH_SMOOTH  
	EL_GROUP       = mesh_smooth_elem  
	CORRECT_ELEMENTS = YES  
	FREE_SF        = FREE
END_

    All free surface nodes may remain free.

  4. To constrain the node displacement to 10, define a Design Variable Constraint (DVCON_SHAPE): 

    DVCON_SHAPE  
	ID_NAME        = DVCON_LIMIT  	
	CHECK_BC       = NO  
	ND_GROUP       = design_nodes 	
	CHECK_GROW     = 10  
	CHECK_SHRINK   = 10
END_

  5. To consider the boundary conditions for the node displacement, define a second Design Variable Constraint (DVCON_SHAPE): 

    DVCON_SHAPE  
	ID_NAME        = DVCON_BC
	CHECK_BC       = YES  
	ND_GROUP       = design_nodes
END_

  6. To constrain the volume, define a Design Response (DRESP) that references the volume of all elements:: 

    DRESP  
	ID_NAME        = DRESP_VOLUME 
	DEF_TYPE       = SYSTEM  
	TYPE           = VOLUME  
	EL_GROUP       = ALL_ELEMENTS
END_

  7. Define an Objective Function (OBJ_FUNC) that references the Design Response and sets the target to MIN:

    OBJ_FUNC  
	ID_NAME        = MINIMIZE_VOLUME  
	TARGET         = MIN  
	DRESP          = DRESP_VOLUME, ,  
END_

  8. To define the stress constraint, do the following;

    1. Create a Design Response (DRESP) for the maximum Mises stresses of the STRESS_NODES node group. 

      DRESP  
	ID_NAME        = DRESP_MAX_MISES  
	DEF_TYPE       = SYSTEM  
	TYPE           = SIG_MISES  
	ND_GROUP       = STRESS_NODES  
	LC_SET         = STATIC,1,All
END_

    2. Reference the Design Response in a constraint (CONSTRAINT), set a relative value of 90% and the constraint type to less or equal: 

      CONSTRAINT  
	ID_NAME        = CONSTRAINT_stress  
	MAGNITUDE      = REL  
	DRESP          = DRESP_MAX_MISES  	
	LE_VALUE       = 0.9
END_

  9. To constrain the frequency, do the following:

    1. Create a Design Response (DRESP) with an Eigenmode of 5: 

      DRESP  
	ID_NAME        = DRESP_FREQ  
	DEF_TYPE       = SYSTEM  
	TYPE           = DYN_FREQ  
	LC_SET         = ALL,10001,5
END_

    2. Reference the Design Response in a constraint (CONSTRAINT),set a relative value of 110% and the constraint type to greater or equal: 

      CONSTRAINT  
	ID_NAME        = CONSTRAINT_freq  	
	MAGNITUDE      = REL  
	DRESP          = DRESP_FREQ  
	GE_VALUE       = 1.1
END_

  10. Reference the Design Variables, Objective Function, constraints and the mesh smoothing in the OPTIMIZE command:

    OPTIMIZE  
	ID_NAME        = SHAPE_OPTIMIZATION  
	OBJ_FUNC       = MINIMIZE_VOLUME  
	DV             = MY_DV_SHAPE  
	DVCON          = DVCON_LIMIT  
	DVCON          = DVCON_BCC  
	CONSTRAINT     = CONSTRAINT_stress  
	CONSTRAINT     = CONSTRAINT_freq  
	MESH_SMOOTH    = MY_MESH_SMOOTH  
	STRATEGY       = SHAPE_SENSITIVITY
END_

    Make sure you chose the SHAPE_SENSITIVITY strategy.

The result looks as follows: