Solution Parameters

Ansys > Running an Analysis > Solution Parameters

XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''">XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''">

Solution Parameters

Linear Static

This subordinate form appears when the Solution Parameter button is selected on the Analysis form when Static is the selected Solution Type.

Nonlinear Static (ANSYS 4.4)

This subordinate form appears when the Solution Parameter button is selected on the Analysis form
when Nonlinear Static is the selected Solution Type and the Preference is set to ANSYS (ANSYS Revision 4.4).

More data input is available for defining the Nonlinear Static Solution Parameters shown on the previous page. Listed below are the remaining parameters contained in this menu.


Input Data	Description
Stepped Boundary Conditions	Causes the analysis to step the boundary conditions rather than ramp them. If selected, this will generate the KBC,1 command.
Large Deflection Analysis	Causes the analysis to include the large deflection option in the solution. This is the KAY,6, 1 command.
Include Stress Stiffening	If selected, this causes the analysis to include the effects of stress stiffening in the analysis. This is the KAY,8, 1 command.
Virtual Wavefront Solution	If selected, this will cause ANSYS 4.4 to select a virtual equation solver for analyses that cannot be solved in-memory. This is the KAY,10, 1 command.

Nonlinear Static (ANSYS 5)

This subordinate form appears when the Solution Parameter button is selected on the Analysis form when Nonlinear Static is the selected Solution Type and the Preference is set to ANSYS 5.

Convergence Criteria

This subordinate form appears when the Convergence Criteria button is selected from the Nonlinear Static Solution Parameters forms and the Preference is set to ANSYS 5.

Advanced Options (ANSYS 4.4)

This subordinate form appears when the Advanced Options button is selected from the Nonlinear Static Solution Parameters forms and the Preference is set to ANSYS (ANSYS Revision 4.4).

Advanced Options (ANSYS 5)

This subordinate form appears when the Advanced Options button is selected from the Nonlinear Static Solution Parameters forms and the Preference is set to ANSYS 5.

Eigenvalue Buckling (ANSYS 4.4)

This subordinate form appears when the Solution Parameter button is selected on the Analysis form
when Eigenvalue Buckling is the selected Solution Type and the Preference is set to ANSYS (ANSYS Revision 4.4).

More data input is available for defining the Eigenvalue Buckling Solution Parameters shown on the previous page. Listed below are the remaining parameters contained in this menu.


Parameter Name	Description
Mode Expansion Procedure	Defines the method to use for expanding modes. Available options are: Expand First Mode Only, Expand No Modes and Expand N Modes. If Expand N Modes is selected, the Number of Modes Databox will be active. This is the KEXPM parameter on the ⁄BUCKLE command.
Number of Modes	This will be active when the Mode Expansion Procedure is set to Expand N Modes. The number entered in this databox will be used as the KEXPM parameter on the /BUCKLE command.
Calculate Buckling Stresses	If selected, this will cause the KPSTR parameter of the /BUCKLE command to be set to 1.
Virtual Wavefront Solution	If selected, this will cause ANSYS 4.4A to select a virtual equation solver for analyses that cannot be solved in-memory. This is the KAY,10, 1 command for ANSYS 4.4A. This option is not displayed if the Selected Preference is “ANSYS 5.”

Eigenvalue Buckling (ANSYS 5)

This subordinate form appears when the Solution Parameter button is selected on the Analysis form when Eigenvalue Buckling is the selected Solution Type and the Preference is set to ANSYS 5.

More data input is available for defining the Eigenvalue Buckling Solution Parameters shown on the previous page. Listed below are the remaining parameters contained in this menu.


Parameter Name	Description
Mode Expansion Procedure	Defines the method to use for expanding modes. Available options are: Expand First Mode Only, Expand No Modes and Expand N Modes. If Expand N Modes is selected, the Number of Modes Databox will be active. If Expand No Modes is the selected procedure, no MXPAND command and no EXPASS command will be written. If Expand First Mode Only is selected, the EXPASS, ON command and the MXPAND command will be written with NMODE set to 1. If Expand N Modes is selected, the EXPASS, ON and MXPAND command will be written. The value of NMODE will be set by the data in the Number of Modes databox.
Number of Modes	Becomes active when the Mode Expansion Procedure is set to Expand N Modes. The number entered in this databox will be used as the NMODE parameter on the MXPAND command.
Calculate Buckling Stresses	If selected, this will cause the ELCALC parameter of the MXPAND command to be set to “YES.” Otherwise, the ELCALC parameter will be set to “NO.”

Modal

This subordinate form appears when the Solution Parameter button is selected on the Analysis form when Modal is the selected Solution Type.

More data input is available for defining the Modal Solution Parameters shown on the previous page. Listed below are the remaining parameters contained in this menu.


Parameter Name	Description
Normalize Shapes 12to Unity	Controls the normalization of the mode shapes. If it is selected, the KPMOD parameter of theKAY,3 command will be set to the negative of the value in the Number of Modes to Print databox for ANSYS 4.4. If ANSYS 5 is being used, this will set the Nrmkey parameter of the MODOP command to ON.
Include Stress Stiffening	If selected, this causes the analysis to include the effects of stress stiffening in the analysis. This is the KAY,8, 1 command for ANSYS 4.4, or the SSTIF, ON command for ANSYS 5.
Virtual Wavefront Solution	If selected, this will cause ANSYS 4.4A to select a virtual equation solver for analyses that cannot be solved in-memory. This is the KAY,10, 1 command for ANSYS 4.4. This option is not displayed if the Selected Preference is “ANSYS 5.”
Expansion Parameters	Brings up the subordinate form to allow definition of the parameters that will control the expansion of the modes. See Mode Expansion Parameters.

Mode Expansion Parameters

This subordinate form appears when the Expansion Parameters button is selected from the Mode/Frequency Solution Parameters form.

Harmonic

This subordinate form appears when the Solution Parameter button is selected on the Analysis form when Harmonic is the selected Solution Type.

More data input is available for defining the Harmonic Solution Parameters shown on the previous page. Listed below are the remaining parameters contained in this menu.


Parameter Name	Description
Output Format	Defines the KPPHA parameter of the KAY,3 command for ANSYS 4.4 or the REIMKY parameter of the HROUT command for ANSYS 5. Options are Amplitude and Phase, or Real and Imaginary (default).
Mass Damping Value	Defines the VALUE parameter of the ALPHAD command.
Stiffness Damping Value	Defines the VALUE parameter of the BETAD command.
Damping Ratio	Defines the RATIO parameter of the DMPRAT command.

Expansion Parameters (Multiple Solutions)

This subordinate form appears when the Expansion Parameters button is selected from the Harmonic Solution Parameters form, and the Method of expansion is set to Multiple Solutions. The Expansion Parameters button can only be selected if the solution method is Reduced.

More data input is available for defining the Multiple Solutions Expansion Parameters shown on the previous page. Listed below are the remaining parameters contained in this menu.


Parameter Name	Description
Phase Angle Options	Defines the KIMG parameter of the /STRESS command for ANSYS 4.4, or the ANGLE parameter of the HREXP command for ANSYS 5. Available options are All or Specify. If All is selected, KIMG is set to 1 for ANSYS 4.4 or ANGLE is set to “All” for ANSYS 5.
Phase Angle Value	Defines the PHASE parameter of the HARFRQ command for ANSYS 4.4 or the ANGLE parameter of the HREXP command for ANSYS 5. This databox is presented only if the Phase Angle Options option menu is set to Specify.
Calculate Stresses and Reactions	Defines the ELCALC parameter of the NUMEXP command for ANSYS 5. It has no effect for ANSYS 4.4.

Expansion Parameters (One Loadstep/Substep)

This subordinate form appears when the Expansion Parameters button is selected from the Harmonic Solution Parameters form, and the Method of expansion is set to One loadstep/substep. The Expansion Parameters button can only be selected if the solution method is Reduced.

Expansion Parameters (Specified Frequency)

This subordinate form appears when the Expansion Parameters button is selected from the Harmonic Solution Parameters form, and the Method of expansion is set to Specified Frequency. The Expansion Parameters button can only be selected if the solution method is Reduced.

Master Degrees of Freedom

This subordinate form appears when the Master Degrees of Freedom button is selected from the Eigenvalue Buckling, Modal/Frequency or Harmonic Solution Parameters forms.

When running a modal analysis with ANSYS Revision 4.4 using Subspace extraction setting the Total Master Degrees of Freedom to 0 (zero) and not selecting any DOF Lists will cause a Full Subspace analysis to be performed. Otherwise, a Reduced Subspace Analysis will be performed.

Steady-State Heat Transfer

This subordinate form appears when the Solution Parameter button is selected on the Analysis form when Steady-State Heat Transfer is the selected Solution Type.

More data input is available for defining the Nonlinear Transient Dynamic Solution Parameters shown on the previous page. Listed below are the remaining parameters contained in this menu.


Parameter Name	Description
Uniform Temperature	Defines the value of the uniform temperature for the analysis. The value here will appear in the TUNIF command.
Reference Temperature	Defines the value of the reference temperature for the analysis. The value here will appear in the TREF command.
Virtual Wavefront Solution	If selected, this will cause ANSYS 4. to select a virtual equation solver for analyses that cannot be solved in-memory. This is the KAY,10, 1 command for ANSYS 4.4. This option is not used for ANSYS 5.