> For the complete documentation index, see [llms.txt](https://dante-solutions-inc.gitbook.io/dante-6.3-help-documentation/llms.txt). Markdown versions of documentation pages are available by appending `.md` to page URLs; this page is available as [Markdown](https://dante-solutions-inc.gitbook.io/dante-6.3-help-documentation/introduction/cylinder-2d-carb-cae.md). # Build Carburization Model using Abaqus-CAE In this section, a gas carburization model of a 2D axisymmetric cylinder is created. The model is built mainly using ABAQUS/CAE. Small amount of editing work on the input file is required. The following is the detailed list of model building steps. ## Step 1: Start ABAQUS/CAE * Start ***ABAQUS CAE*** using command: ***abaqus cae*** under ABAQUS command window. The ABAQUS ***Start Session*** window pops up.

* Click ***With Standard/Explicit Model*** to start a new model. ## Step 2: Create a Part * Select ***Part*** module to create the part geometry.

* ***Create Part***, give the part name as ***cylinder-2d***. Check ***Axisymmetric*** for Modeling Space. Using defaults for all others.

* Click ***Continue*** to sketch the part geometry. The cylinder’s diameter is 30 *mm*, and its length is 80 *mm*. Half cross section (rectangular) is used to model the heat treatment process. The four corner coordinates of the rectangular are (0,0), (15,0), (15,80), (0,80) respectively. ***Create Lines: Connected*** is used to sketch the geometry. Click ***Done*** when geometry sketching is done. The figure of the geometry is shown below.

***Note: To model axisymmetric geometry, y-axis will be used as symmetric axis automatically.*** * Save the pre-processing file as: ***cylinder-2d***. (cylinder-2d.jnl and cylinder-2d.cae files will be saved to the working directory) ## Step 3: Meshing the Part * Select ***Assembly*** module.

* ***Instance*** \ ***Create,*** the following window pops up.

* Click ***Ok*** to create an instance. * Select ***Mesh*** module to mesh the part. Check ***Part*** instead of ***Assembly***.

***Note: This model is going to simulate the carburization process. Fine surface meshing is required to catch the accuracy. Partition of the geometry is used to obtain fine surface mesh.*** * ***Tools*** \ ***Partition***, select ***Face, Sketch*** options as the following figure, and click ***OK***.

* Using ***Offset Curves*** for the partition. Select the three edges outside.

* Make the thickness of the surface layer ***1.5 mm*** for accurately catch the carbon gradient and thermal gradient. * After partition, the part should look like the figure below.

* Give a reasonable element seeds, using the figure below as reference. ***Seed*** \ ***Part*** to set global element size 1.0

***Seed*** \ ***Edge by Number*** to seed all the surface edges.

Click ***Done*** when all the edges are seeded. * A figure is shown below after applying seeds.

* ***Mesh*** \ ***Controls***, box select the whole part geometry by dragging the mouse, and click ***Done***.

* A small window appears. Select ***Quad***, ***Structured*** element. Click ***OK*** and the part color should be green. Click ***Done*** to exit ***Mesh Controls***.

* ***Mesh*** \ ***Element Type***. Box select the whole region, and click ***Done***. ***Element Type*** window appears. Select ***Standard***, ***Linear***, ***Heat transfer*** element for mass diffusion. Click ***OK***. Click ***Done*** to exit Assigning Element type.

* ***Mesh*** \ ***Part*** to mesh the part. Click ***Yes*** to mesh the part. A mesh figure (top of the model) is shown below.

## Step 4: Create Material Properties * Select ***Property*** module to define the material properties. * ***Material / Create***, the ***Edit Material*** window shows up. * Set the name as material: **STEEL\_*****S41XX***. Note: S41XX is a specified material name in DANTE database, and prefix “STEEL\_” is needed to make the difference from Aluminum and Nickel alloys/ * Define the ***Density*** property.

The material properties include: ***General*** / ***Density***: 7.86E-06 * ***Section*** / ***Create*** to create a section. Select ***Solid*** , ***Homogeneous***

* Click ***Continue***, Select STEEL\_***S41XX*** from material option. Click ***OK*** to exit

* ***Assign*** / ***Section*** to assign the section to the model * Select the whole region to ***assign the section (material) to all the elements***.

* ***Assign Section*** window appears. Click ***OK*** to finish the assigning. The color of the part should change.

## Step 5: Create Simulation Steps * Select ***Step*** module. * ***Step*** / ***Create***, and Create Step window appears. Name the step as ***carburizing*** (optional). Select ***Heat transfer*** and click ***Continue***.

* ***Edit Step*** window appears. Total carburizing time period: ***21600*** seconds.

* Define the ***Incrementation*** as the figure below, and click ***OK*** to exit.

Note: \*Step definition can be modified by editing the input deck. ## Step 6: Define Output Requests * ***Output*** / ***Restart Requests*** to manage the restart file. Specify the frequency, and click ***OK*** to exit. Note: A frequency of 1 will write out a large restart file

* ***Tools*** / ***Set*** / ***Create*** to define a node set for monitor. Set name: ***Monitor\_Node***. Click ***Continue***

* Select a point from the region to be the monitor node. Click ***Done*** * ***Output*** / ***DOF Monitor***, select the pre-defined node set “***Monitor***” for the Region definition. Specify the ***Degree of freedom***: 11. Click ***OK*** to exit.

* ***Output*** / ***Field Output Requests*** / ***Manager*** / ***Edit***. ***Edit Field Output Request*** window appears. Select the Thermal output (***NT***). Write output frequency as ***10***. Click ***OK*** to exit.

***(Optional)*** * Create a node set for history output. ***Tools*** / ***Set*** / ***Create***, select the whole region to define a node set as ***all\_node***. * ***Output*** / ***History Output Requests*** / ***Create*** to define history output. ## Step 7: Define Boundary Conditions * Select ***Interaction*** module to define the carburizing boundary potentials. * ***Interaction Create***, and ***Create Interaction*** window appears. * Select ***Surface film condition***, and click ***Continue***. (Convection is used to mimic the carbon reaction on part surface)

* Select the entire exposed surface of the part to impose the carburizing atmosphere Note: using **Shift + Click** for multiple selection. * Set the magnitude as ***0.008*** (0.8% carbon). Click ***OK*** to exit

* Go to the ***Load*** module, to define the base carbon of the material. * ***Predefined Field*** / ***Create*** to define the part initial carbon. Select ***Initial*** step, ***Other*** / ***Temperature***, and box select the entire part.

* In the ***Edit Predefined Field*** window, assign a value of ***0.002***, and click ***OK***. The material has 0.2% carbon as initial condition. * ***Predefined Field*** / ***Create*** to define the carburization temperature using the first field variable.

* ***Create Predefined Field*** window shows up. Select ***carburization*** step, check ***Other***, and select ***Field***.

* Click ***Continue***, and box select the entire part. Click ***Done*** * ***Edit Predefined Field*** window shows up. Set ***Magnitude*** to ***900°C*** as the initial temperature, Click ***OK*** to exit.

## Step 8: Write Out Input File * Select ***Job*** module. * ***Job*** / ***Manager***, and ***Job Manager*** window appears.

* Click ***Create*** to create a new job. ***Create Job*** window appears. Give the job name as ***cylinder\_2d\_gas\_c*** (optional).

* Click ***Continue*** and ***Edit Job*** window appears. Select the default options. Click ***OK*** to exit.

* In the ***Job Manager*** window, click ***Write Input*** to write out the input deck. The input file name is ***cylinder\_2d\_gas\_c.inp***.

## **Step 9:** **Modifying Carburizing Input File** * **User material should be used.** ***Change from*** ``` *Material, name=STEEL_S41XX *Density 7.83e-06, ``` ***to:*** ``` *Material, name=STEEL_S41XX *Density 7.83e-06, *Depvar 5, 1, Temperature, Carburizing Temperature 2, CRBALL, Carbon All 3, ALLOYPPT, Volume Fraction of Alloy Precipitate 4, ALLOYPPT_SIZE, Alloy Precipitate Size 5, CARBON, Nascent Carbon Weight Fraction *User Material, constants=2, type=THERMAL 7.83e-06,-1. ``` Notes: 1\) Five (5) Solution Dependent Variables (SDV) are need for carburizing model. 2\) The second material constant needs to be “-1” for carburizing model. **Editing the output results if necessary.** ``` *Output, field, frequency=10 *Node Output NT, *Element Output, directions=YES SDV1,SDV2,SDV3,SDV4,SDV5 ** ****************************************************************** ``` * **Start the simulation using the following command** **abaqus job=cylinder\_2d\_gas\_c \[cpus=X]** ## **Step 10:** **Create Carbon Content File for Thermal and Stress Analysis** After running the carburization model, the carbon distribution contour can be plotted using ***ABAQUS Viewer***.

The carbon distribution file is required for thermal and stress models. This file can be obtained from ***ABAQUS/Viewer*** post-process. The format of the file needs to be edited. · ***Report / Field Output***, the ***Report Field Output*** window pops up. Select ***Unique Nodal***, ***SDV\_CARBON*** (or NT11) under variable tab.

· Under setup tab, give the file name as ***cylinder\_2d\_gas\_cc.cbn***. Make sure to select the last frame. Click OK to write the carbon distribution file to the working directory.

During thermal and stress analysis, the carbon content at each node is read in through a file using card: ``` *Field, OP=NEW, VAR=1, Input=cylinder_2d_gas_cc.cbn ``` The cylinder\_2d\_gas\_cc.cbn file format is given as follow: ``` INSTANCE_NAME. NODE, CARBON Value ```

**Note: non data line should be commented out by “\*\*”**