The abaqus moldflow translator reads the Moldflow interface files and creates the relevant files. The files created depend on which options you include on the command line when executing the translator. For a midplane simulation the abaqus moldflow translator creates a partial Abaqus input file, a neutral file, and an initial stress file. # Partial Abaqus input (.inp) file The partial Abaqus input file contains model data consisting of nodal coordinates, element topology, and section definitions. It also contains a \*STATIC step with default output requests. If you are working with isotropic materials, the input file contains material property data. Each input file begins with a series of comments that summarize the data provided by the Moldflow interface files and how the data are translated to the Abaqus input file. Additional data, such as boundary conditions and loads, and nondefault output requests must be added to this file manually. # Neutral (.shf) file containing material data for layered, spatially varying material properties Material data are translated into an appropriately formatted ASCII neutral file. This file contains lamina material property data for each layer of each element. The Abaqus \*ELASTIC, TYPE=SHORT FIBER and \*EXPANSION, TYPE=SHORT FIBER options in the Abaqus input file direct Abaqus/Standard to read material data from this file during the initialization step. # Data lines in the neutral file: First line: 1. Number of elements in the .shf file. 2. Number of layers in each shell section. Subsequent lines: 1. Element label. 2. Layer identifier. 3. $E _ { 1 }$ 4. $E _ { 2 }$ 5. . $\nu _ { 1 2 }$ 6. $G _ { 1 2 }$ 7. $G _ { 1 3 }$ 8. $G _ { 2 3 }$ 9. $\alpha _ { 1 }$ 10. $\alpha _ { 2 }$ 11. Fiber orientation angle (in degrees), measured relative to the default element orientation. This data line is repeated as often as necessary to define the above parameters for different layers of a shell section within different elements. # Initial stress (.str) file Residual stress data from the Moldflow analysis are translated into an appropriately formatted ASCII neutral file. These data are defined in terms of the local Abaqus coordinate system at each section point. The Abaqus \*INITIAL CONDITIONS, TYPE=STRESS, SECTION POINTS option in the Abaqus input file directs Abaqus/Standard to read initial stress data from this file during the initialization step. # Files created for a three-dimensional solid simulation The abaqus moldflow translator reads the Moldflow interface files and creates the relevant files. The files created depend on which options you include on the command line when executing the translator. If you are using an unfilled model, the abaqus moldflow translator creates only the partial Abaqus input file described below. For a three-dimensional solid simulation using a filled model, the translator may create additional files, as described below. # Partial Abaqus input file The partial Abaqus input file contains model data consisting of nodal coordinates, element topology, and section definitions. Additional data, such as service loads and boundary conditions, and nondefault output requests must be added to this file manually. Boundary condition data sufficient to remove rigid body modes are also included. # Material (.mpt) file containing orthotropic material properties data Material data from the Moldflow analysis are collected and placed in a binary file. The data written to the file are in the same form as the information provided for the Abaqus \*ELASTIC, TYPE=ENGINEERING CONSTANTS option. These are defined in terms of the local Abaqus coordinate system of each element. # Orientation (.opt) file containing element orientation data Orientations defining the directions for material properties and initial stresses are computed and placed in this binary file. # Thermal expansion (.tpt) file containing element thermal expansion coefficient data The orthotropic thermal expansion data from the Moldflow analysis are collected and placed in a binary file. These are defined in terms of the local Abaqus coordinate system of each element. # Preparing the Abaqus input file for analysis Once the abaqus moldflow translator has created the Abaqus input file, you must complete the input file manually before submitting it for analysis (see “Defining a model in Abaqus,” Section 1.3.1, for details). # Preparing for a shrinkage and warpage analysis A shrinkage and warpage analysis calculates the deformation caused by the residual stresses in the model after it is removed from the mold. Usually only rigid body modes must be removed. In this case you must ensure that residual stresses have been translated. For three-dimensional solid Moldflow simulations boundary conditions sufficient to restrain rigid body modes are automatically translated to the input file. In other cases you are required to add appropriate boundary conditions to remove the rigid body modes of the model. In certain cases problems with convergence can occur when you must account for geometric nonlinearity and large initial stresses are present. You can overcome these problems by using two analysis steps: • In the first step constrain all displacement degrees of freedom. • In the second step use the OP=NEW parameter to apply boundary conditions that remove the rigid body modes. # Preparing for a service loading analysis A service loading analysis (with appropriate boundary conditions) assesses the performance of the model. You can perform this analysis with or without initial stresses. You must specify the appropriate boundary conditions and loads as history data in the Abaqus input file. # Preparing for other analysis types Any Abaqus/Standard analysis procedure can be performed with the translated model provided that you specify the correct boundary conditions and loading in the Abaqus input file. In addition, certain analysis types may require you to specify additional material constants, model data, and/or solution controls in the input file. # Command summary abaqus moldflow ```ini job=job-name [input=input-name] [midplane | 3D] [element_order={1 | 2}] [initial_stress={on | off}] [material=traditional] [orientation=traditional] ``` # job This option specifies the input and output file names to use during results translation. The job-name value is used to construct the default SIM database file name, job-name.sim. The output modal neutral file is given the name job-name.mnf. If this option is omitted from the command line, the user will be prompted for this value. # input This option is used to specify the name of the files containing the Moldflow interface data if it is different from job-name. # midplane This option is used to translate the results of a midplane simulation to an Abaqus model with threedimensional (shell) elements. # 3D This option is used to translate the results of a three-dimensional solid simulation to an Abaqus model with solid elements. # element\_order This option is used to specify the order of elements created in the partial input file for three-dimensional solid simulations. Possible values are 1 to create first-order elements (C3D4) and 2 to create secondorder elements (C3D10). The default value is 2. This option is valid only when using the 3D option. # initial\_stress This option specifies whether or not initial stress will be included in the model. This option is valid only when using the 3D option. If the initial\_stress option is not included or if initial\_stress=off, initial stresses will not be translated. If initial\_stress=on, initial stresses will be written to the input file. # material This option is used to specify where the material properties are written. If material=traditional, the material properties will be written to the input file. Otherwise, the material properties will be written to the (binary) .mpt file. Using material=traditional is not recommended for large models for performance reasons since every element will have its own \*MATERIAL definition. # orientation This option is used to specify where the orientations are written. If orientation=traditional, the orientations are written to the input file. Otherwise, the orientations will be written to the (binary) .opt file. Using orientation=traditional is not recommended for large models for performance reasons since every element will have its own \*ORIENTATION definition. # 3.2.42 ENCRYPTING AND DECRYPTING Abaqus INPUT DATA Products: Abaqus/Standard Abaqus/Explicit # References • “Execution procedure for Abaqus: overview,” Section 3.1.1 • “Including an encrypted data file” in “Defining a model in Abaqus,” Section 1.3.1 • \*INCLUDE # Overview You can use the abaqus encrypt utility to prevent the unauthorized use of Abaqus input data. The utility converts a data file into an encrypted, password-protected format that only authorized Abaqus input parties can access. The utility is intended for the encryption of data that you include by reference in input (.inp) files or in other data files. For example, you could encrypt a file that contains all of the proprietary material data for your model, then include the encrypted data file by reference in an unencrypted Abaqus input file. See “Including an encrypted data file” in “Defining a model in Abaqus,” Section 1.3.1, for information on how to include an encrypted data file in an Abaqus input file. You can encrypt any input file. However, Abaqus cannot run an encrypted Abaqus input file directly; the encrypted file must be included in an unencrypted file. You cannot use parameterized input in the encrypted file. # Specifying additional access levels and controls You can customize your encryption so that only users with a license for a particular Abaqus feature or from a particular site can include or decrypt the file. For example, you can specify that only Abaqus/Standard users can access the file. You can also prevent decryption of an encrypted file by any user, regardless of their license and site; end users can still use the encrypted data in an analysis by including it by reference in an unencrypted Abaqus input file, provided that the users know the encrypted file’s password. # Security and support considerations The primary intent of the Abaqus encryption implementation is to prevent unauthorized use of encrypted input data, not to prevent disclosure of encrypted data to authorized users. Running an Abaqus analysis input using encrypted data may produce output files that are not encrypted. Only material and connector behavior information contained within an encrypted input file is prevented from being visible in the output. This approach means that recipients of encrypted data who satisfy the access criteria, such as the password, license feature, or SiteID, will be able to reconstruct some input in an unencrypted form. Providers of encrypted data should consider establishing contractual agreements to protect proprietary data. Users of encrypted data must accept responsibility for security of files produced from encrypted input and should consider restricting access to resulting analysis files. Abaqus technical support cannot retrieve lost passwords for encrypted data files. Users receiving encrypted data should contact the data provider for any technical support issues. # Adding comments to the header of an encrypted file When you encrypt a file, Abaqus adds the following unencrypted comment line to the beginning of the file: # \*\* encrypted input Do not modify or delete this header comment. You can, however, insert additional comment lines between this header comment and the first line of encrypted data. These post-encryption comment lines can describe the encrypted file’s contents, provide release numbers, or display copyright and legal information about the encrypted data. For more information about comment line syntax, see “Input syntax rules,” Section 1.2.1. You should not, however, add post-encryption comment lines within the lines of encrypted data. If you want to edit or amend the comment lines within the data itself, you must first decrypt the data. Command summary

abaqus {encrypt | decrypt}

input=input-file-nameoutput=output-file-namepassword=password[license=feature_list][expiration=expiration_date]

[siteid=site-id_list]

[include_only]

# Command line options # input This option specifies the name of the data file that you want to encrypt or decrypt. If you omit this option from the command line, Abaqus will prompt you for its value. # output This option specifies the name of the data file after encryption or decryption. If you omit this option from the command line, Abaqus will prompt you for its value. # password This option specifies the password for this encryption or decryption. Passwords are case-sensitive. If you omit this option from the command line while encrypting data, Abaqus will prompt you for its value. If you enter the password incorrectly or omit it from the command line while decrypting data, Abaqus reports that the input file is either corrupted or the password is incorrect. # license This option applies only to file encryption. This option specifies the Abaqus feature or features for which end users must be licensed if they want to include or decrypt this encrypted data file. You can use a comma-separated list to allow access to the file by licensees of any one of a series of Abaqus features. Any feature name that appears in an Abaqus license file is valid. These might include the following features: foundation, standard, explicit, design, aqua, ams, cae, viewer, cae\_nogui, cmold, moldflow, safe, cadporter\_catia, cadporter\_catiav5, cadporter\_ideas, cadporter\_parasolid, cadporter\_proe, afcv5\_structural, and afcv5\_thermal. # siteid This option applies only to file encryption. This option specifies the Abaqus Site ID or IDs where end users can include or decrypt this encrypted data file. You can use a comma-separated list to allow multiple sites access to the file. You can use this option only when you also use the license option. To determine your Abaqus Site ID, run abaqus whereami from a command prompt. # include\_only This option applies only to file encryption. This option specifies that encrypted input data cannot be decrypted using the abaqus decrypt execution procedure; such data can only be included in an Abaqus input file. If you attempt to decrypt a file that was encrypted with the include\_only option, Abaqus issues an error message stating that the input file can be included in an analysis but is not eligible for decryption. # expiration This option applies only to file encryption. This option specifies the date after which the end users can no longer decrypt or include the encrypted data file. The date must be provided in the formYYYY-MM-DD. # Examples The following examples illustrate the different encryption methods that are possible using the encrypt execution procedure. # Creating encrypted files In the simplest encryption scenario an Abaqus user creates an encrypted copy of a file named material\_data.inp, which contains all of the material data for a model, before sending the encrypted version to an authorized end user. Encryption prevents unauthorized users from accessing the encrypted file during its transmission. To create an encrypted copy of material\_data.inp named material\_data\_enc.inp, issue the following command: ```txt abaqus encrypt input=material_data.inp output=material_data_enc.inp password=e1No9c2z ``` Upon receiving the file, the end user can run the abaqus decrypt execution procedure to create a copy of the original, non-encrypted material data file. Because of the encryption options selected in this example, the end user requires only the encrypted file’s password to decrypt it. To decrypt the encrypted data file material\_data\_enc.inp, producing the non-encrypted file material\_data.inp, issue the following command: ```txt abaqus decrypt input=material_data_enc.inp output=material_data.inp password=e1No9c2z ``` Alternatively, the end user can skip the decryption and run an analysis that includes the encrypted data by reference. To include the encrypted file by reference in an Abaqus input file, add the following statement to the input file: ```python *INCLUDE, INPUT=material_data_enc.inp, PASSWORD=e1No9c2z ``` # Limiting access to decrypted files by license feature or site ID You can specify that end users cannot access the file unless they have a valid license for a particular Abaqus feature, run Abaqus at a particular site, or satisfy both of these criteria. To encrypt a data file that can be accessed only by users who have an Abaqus/Explicit license and who run the software at site 09YYY, issue the following command: ```txt abaqus encrypt input=material_data.inp output=material_data_enc.inp password=e1No9c2z license=explicit siteid=09YYY ``` An end user can attempt to access the file material\_data\_enc.inp using the same decryption or inclusion syntax specified in the previous example. For this encrypted file, Abaqus would validate that the end user has an Abaqus/Explicit license and is running Abaqus at site 09YYY before providing access to the file. If the end user’s license or site settings do not match those specified during encryption, Abaqus issues an error message that lists the licenses or sites that are required to access the file. # Creating encrypted files that must be included to be used by Abaqus You can use the include\_only option to prevent end users from decrypting the file directly using abaqus decrypt. Authorized users can access a file encrypted with the include\_only option by including the file by reference in an Abaqus input file. Material and connector behavior definitions within an encrypted input file are not written to the output database. In addition, all material and connector behavior definitions output to the data file are suppressed if an encrypted file is used as input for any portion of the model. To create an encrypted file that is available only for inclusion by reference in other input files, issue the following command: ```txt abaqus encrypt input=material_data.inp output=material_data_enc.inp password=e1No9c2z include_only ``` The resulting encrypted file can be included by reference in an Abaqus input file using the same syntax as in the previous example. If you attempt to decrypt a file that was encrypted with the include\_only option, Abaqus returns an error message.