The Custom Results command will allow you to create a new result which can be plot as a contour on the model. This new result can be based on material properties, element properties and current results. Selecting this command will access the Calculation dialog. The basic process for creating a custom result consists of 5 steps.
- Name a new custom result or select an existing custom result: When the Calculation dialog is accessed, the New Calculation option will be selected in the Name: drop-down box. Clicking in the drop-down box will allow you to type a descriptive name for the custom result. This name will appear in the Custom Results drop-down menu. All previously defined custom results will also be listed in this drop-down box.
- Name the variables to be used in the custom result calculation: The table in the center of the dialog lists the variables that will be used to calculate the custom result. To add a variable, select a blank row in the table. Clicking in the Name column will allow you to type a name for the variable. Note: Variable names may contain any alphanumeric characters or the '_' character. Variable names cannot contain spaces. The first character in the name must not be a number. Variable names are case sensitive.
- Define the variables: There are three ways to define a variable. These can be accessed by right-clicking on the row for the variable.
- Results for Active Window: This pull-out menu reflects many of the commands available on the Results Contours tab. Select the value that will be used for the selected variable. Most of the values are scalar. Selecting the Vector Plot option when available will select the 3D vector.
- Results for Analysis Type: This pull-out menu contains all the result types that are available for the current analysis type. These values include scalar, vector and tensor values. The meaning of most of the commands in this menu is apparent. The Position command will provide the X, Y and Z coordinates of the nodes at the beginning of the analysis.
- AGSDB Query: Properties from model database can be accessed using the Autodesk Simulation General Simulation Database (AGSDB). Values can be selected from the model.dbf file for the model. This can be used to include material properties in the custom result calculations. This command will access the AGSDB Query dialog where you enter the database variable. The variables /p and /e can be used as substitutions for part number and element property ID respectively. For example, to use the modulus of elasticity for each part in a custom result, you can define a variable to be Material(/p).Linear.Isotropic.Emodulus.
Each variable has the following properties associated with it
- Value: This is the general result category. Examples values are displacement and stress. This property will be defined automatically when the variable is defined and cannot be modified.
- Operations: This is subset of the value. Examples operations are magnitude for displacement values and maximum principal for stress values. This property will be defined automatically when the variable is defined. However, the operation can be modified. For most value and operation combinations, the absolute value operation can be added by right-clicking on the variable row in the table and selecting the Add Operator: Absolute Value command. The operators can be removed from a variable, by right-clicking on the variable row in the table and selecting the Clear Operator(s) command. After the operators are removed, a new operator can be added by right-clicking on the variable row in the table and selecting a command in the Add Operator pull-out menu.
- Type: There are two types of results available: scalar and 3D vector. This property will be defined automatically when the variable is defined and cannot be modified.
- Defined At: There are four possible values for this property. Nodal refers to results that are calculated at each node in the model. Element-Nodal refers to results that have a result for each element that shares the node. Element-Face refers to results that are calculated for each face of an element. Element refers to results that are calculated at the centroid of each element. This property will be defined automatically when the variable is defined and cannot be modified.
- Units: This lists the units that are used for the variable based on the model's unit system. This property will be defined automatically when the variable is defined and cannot be modified.
Variables can be deleted by right-clicking on the row in the table and selecting the Delete Variable command.
- Create the formula: Type in the formula for the custom result the field at the bottom of the dialog. The variable names are case sensitive, therefore they must match the names in the table exactly. Scalar values may be entered as bare values or in curly braces, for example,1.23 or {1.23}. Vectors are entered as a sequence of three expressions in curly braces separated by the list separator for the current locale, {1,2,3}. Tensors are entered as a sequence of six expressions in curly braces separated by the list separator for the current locale, for example {1,2,3,4,5,6}. The table below lists the possible functions for scalar, vector and tensor values. Scalars can be combined with vectors and tensors in some situations. x*y will be valid if either x or y is a scalar. x/y will be valid if y is a scalar. If the result of a calculation for any area of the model is not a finite real number, that part of the model will not be shaded. If the result of a formula is a vector or tensor, a pullout menu will appear with the scalarized value. Vector results can also be plotted as a vector field.
Different result types can be combined in the formula. For example if a nodal result is combined with an element-nodal result, the result will be an element nodal result. When the Apply button is pressed, the result type for the entire formula will be displayed in a text string below the Name: drop-down box.
Note: It is not possible to combine a nodal result with an element-face result. If this combination is made, an invalid warning will appear and the result will not appear in the Custom Results drop-down menu.Vector Operations (x and y are vector variables) -x negative value x+y addition x-y subtraction x*y cross product x.y dot product x^y exponent UOpVectorX(x) X component UOpVectorY(x) Y component UOpVectorZ(x) Z component UOpVectorMagnitude(x) magnitude Scalar Operations (x and y are scalar variables) -x negative value x! factorial x+y addition x-y subtraction x*y multiplication x/y division x^y exponent sin(x) sine cos(x) cosine tan(x) tangent asin(x) arcsine acos(x) arccosine atan(x) arctangent sinh(x) hyperbolic sine cosh(x) hyperbolic cosine tanh(x) hyperbolic tangent asinh(x) hyperbolic arcsine acosh(x) hyperbolic arccosine atanh(x) hyperbolic arctangent abs(x) absolute value ln(x) natural log log(x) log base 10 exp(x) exponential sqr(x) square root logn(x,n) log base n rootn(x,n) nth root Tensor Operations (x and y are vector variables) -x negative value x+y addition x-y subtraction UOpTensor11(x) Tensor 11 value UOpTensor22(x) Tensor 22 value UOpTensor33(x) Tensor 33 value UOpTensor12(x) Tensor 12 value UOpTensor23(x) Tensor 23 value UOpTensor31(x) Tensor 31 value UOpVonMises(x) von Mises UOpTresca2(x) Tresca*2 UOpMinimumPrincipal(x) Minimum principal UOpIntermediatePrincipal(x) Intermediate principal UOpMaximumPrincipal(x) Maximum principal UOpMinPrincipalDirection(x) Minimum principal direction UOpIntPrincipalDirection(x) Intermediate principal direction UOpMaxPrincipalDirection(x) Maximum principal direction - Press the Apply button: If the formula is valid, the result type will appear below the Name: drop-down box and the result will appear at the bottom of the Custom Resultsdrop-down menu. The Custom Resultsdrop-down menu can be accessed without exiting the Calculation dialog. If you make changes to the variables or formula, you will need to press the Apply button and select the result command again in the drop-down menu in order for the display contour to be updated. Also, if you make changes to an existing custom result, you must press the Apply button before switching to a custom result in the Name: drop-down box in order for the changes to be saved.
Once a custom result is created, it will appear in the Custom Results drop-down menu for all analyses that have the necessary data available. Custom results can be deleted by selecting the result in the Name: drop-down box and selecting the Delete button.
Note: The calculation will not appear in the Custom Results drop-down menu unless the all the Values used in the calculation exist for the model. For example, if the formula uses stresses but you are viewing the results of a model that does not have stresses (thermal analysis, modal analysis, and so on), the calculation will not be listed in the Custom Results drop-down. Another example is a calculation that uses the volume of the elements. Since the volume result is created by the Weight and Center-of-Gravity tool (Analysis
Analysis Weight And Center-of-Gravity), any calculation that uses volume would not appear in the Custom Results drop-down unless the Weight And Center-of-Gravity tool had been used.
Analysis Weight And Center-of-Gravity), any calculation that uses volume would not appear in the Custom Results drop-down unless the Weight And Center-of-Gravity tool had been used. Attention: Units will not be displayed in the legend box for custom results contours. The custom results are not converted based on the active Display Units. The same equation is used for all models regardless of the units. For example, if a custom result is created for a model or Display Units set to English units, and if the equation contains constants that are in English units, these constants will not be converted when using the custom result with a model or Display Units set to SI units.