> 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.

<figure><img src="/files/VPPdNP9Aeu1m58ZWg76x" alt="" width="518"><figcaption></figcaption></figure>

* Click ***With Standard/Explicit Model*** to start a new model.

## Step 2: Create a Part

* Select ***Part*** module to create the part geometry.

<figure><img src="/files/1Y6z0kMjEewXN9LATfMy" alt="" width="160"><figcaption></figcaption></figure>

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

<figure><img src="/files/oMpIW9AB1sc2CR6wSA1P" alt="" width="230"><figcaption></figcaption></figure>

* 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.

<figure><img src="/files/dFb5yIDDZ1lz9CcrvgZC" alt="" width="80"><figcaption></figcaption></figure>

***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.

<figure><img src="/files/DGYNecXkKBFGcOeubFSX" alt="" width="161"><figcaption></figcaption></figure>

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

<figure><img src="/files/2bDiqs0izwDU1v0vpfYk" alt="" width="371"><figcaption></figcaption></figure>

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

<figure><img src="/files/A4G3BO5SjC97rMJgGUEA" alt="" width="561"><figcaption></figcaption></figure>

***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***.

<figure><img src="/files/P9peEolRnFnT7BB1Oe6c" alt="" width="359"><figcaption></figcaption></figure>

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

<figure><img src="/files/Lk1yf2RF5jnPqivrTC1l" alt="" width="107"><figcaption></figcaption></figure>

* 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.

<figure><img src="/files/HlxWnngPrG8wKlIkA3qY" alt="" width="73"><figcaption></figcaption></figure>

* Give a reasonable element seeds, using the figure below as reference.

***Seed*** \ ***Part*** to set global element size 1.0

<figure><img src="/files/yZqWfbfvwpaLiSoRO54t" alt="" width="381"><figcaption></figcaption></figure>

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

<figure><img src="/files/MQqhX0PQcNkhCYbiop4T" alt="" width="482"><figcaption></figcaption></figure>

Click ***Done*** when all the edges are seeded.

* A figure is shown below after applying seeds.

<figure><img src="/files/CnTi0zM3QbYHjU9ZPAuN" alt="" width="563"><figcaption></figcaption></figure>

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

<figure><img src="/files/dDdv2MwZDfyZrACiWooP" alt="" width="353"><figcaption></figcaption></figure>

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

Click ***Done*** to exit ***Mesh Controls***.

<figure><img src="/files/5q0Bt0qpw45A7J3I5oeu" alt="" width="520"><figcaption></figcaption></figure>

* ***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.

<figure><img src="/files/vCoiacEHfROyyxwnVQVb" alt="" width="563"><figcaption></figcaption></figure>

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

<figure><img src="/files/oMtq1IIQjSoRAxWClJAq" alt="" width="563"><figcaption></figcaption></figure>

## 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.

<figure><img src="/files/CuMzZN8QKJf2OHhnRq1f" alt="" width="396"><figcaption></figcaption></figure>

The material properties include:

***General*** / ***Density***: 7.86E-06

* ***Section*** / ***Create*** to create a section. Select ***Solid*** , ***Homogeneous***

<figure><img src="/files/bMBfHRmv1J0zfzJzSchM" alt="" width="249"><figcaption></figcaption></figure>

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

<figure><img src="/files/3fdJm4oaNWuQBfmI1lrO" alt="" width="245"><figcaption></figcaption></figure>

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

<figure><img src="/files/t3skmpF6MOx0Xsk0mtha" alt="" width="296"><figcaption></figcaption></figure>

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

<figure><img src="/files/3amFaMyckyHqjJy4wit9" alt="" width="84"><figcaption></figcaption></figure>

## 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***.

<figure><img src="/files/PGzRgVnkj3loHo9R4GyD" alt="" width="225"><figcaption></figcaption></figure>

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

<figure><img src="/files/4a37a4Eedy7yoICSQjUr" alt="" width="552"><figcaption></figcaption></figure>

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

<figure><img src="/files/F4Z8DCTygK2lPHU7mdxS" alt="" width="563"><figcaption></figcaption></figure>

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

<figure><img src="/files/7wsnPKiEEutGnKFyAG7h" alt="" width="462"><figcaption></figcaption></figure>

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

<figure><img src="/files/BLadvS1xIsVJ43XRmQN2" alt="" width="295"><figcaption></figcaption></figure>

* 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.

<figure><img src="/files/DnpdpNrsKylZnd2nl0HP" alt="" width="323"><figcaption></figcaption></figure>

* ***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.

<figure><img src="/files/32sNM1YD3T7TsPWSC6Ag" alt="" width="555"><figcaption></figcaption></figure>

***(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)

<figure><img src="/files/O99xnclCJZbiXBCsQojt" alt="" width="341"><figcaption></figcaption></figure>

* 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

<figure><img src="/files/6VtX2Twhb56zBgSvQQ3C" alt="" width="378"><figcaption></figcaption></figure>

* 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.

<figure><img src="/files/0IbxIx9rgEfxC77oEln9" alt="" width="295"><figcaption></figcaption></figure>

* 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.

<figure><img src="/files/5pTdUByUw0C6CS4GZRTM" alt="" width="327"><figcaption></figcaption></figure>

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

<figure><img src="/files/PNO6kEx3TXfNMHDGfCdQ" alt="" width="231"><figcaption></figcaption></figure>

* 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.

<figure><img src="/files/XuvX6DWaM8bu4pw8WMwU" alt="" width="398"><figcaption></figcaption></figure>

## Step 8: Write Out Input File

* Select ***Job*** module.
* ***Job*** / ***Manager***, and ***Job Manager*** window appears.

<figure><img src="/files/AeIjuVInHZAS5nU1PPRq" alt="" width="368"><figcaption></figcaption></figure>

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

<figure><img src="/files/bA9JDPzcil9Z4bRJux3C" alt="" width="347"><figcaption></figcaption></figure>

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

<figure><img src="/files/yKHC6JWqngMlk9RWGAFT" alt="" width="308"><figcaption></figcaption></figure>

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

<figure><img src="/files/NxoYEDq1Wncm0LsNsTQd" alt="" width="461"><figcaption></figcaption></figure>

## **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***.

<figure><img src="/files/IpcyalXQp0Z22xvAnm1z" alt="" width="147"><figcaption></figcaption></figure>

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.

<figure><img src="/files/efcqcbMOqrrGFSdVz6We" alt="" width="344"><figcaption></figcaption></figure>

· 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.

<figure><img src="/files/ZpQEpBMhPwJfqyRSj6ee" alt="" width="516"><figcaption></figcaption></figure>

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
```

<figure><img src="/files/gPP7b2H74lXSHnCA3rdg" alt="" width="473"><figcaption></figcaption></figure>

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


---

# Agent Instructions
This documentation is published with GitBook. GitBook is the documentation platform designed so that both humans and AI agents can read, navigate, and reason over technical content effectively. Learn more at gitbook.com.

## Querying This Documentation
If you need additional information that is not directly available in this page, you can query the documentation dynamically by asking a question.

Perform an HTTP GET request on the current page URL with the `ask` query parameter, and the optional `goal` query parameter:

```
GET https://dante-solutions-inc.gitbook.io/dante-6.3-help-documentation/introduction/cylinder-2d-carb-cae.md?ask=<question>&goal=<endgoal>
```

`ask` is the immediate question: it should be specific, self-contained, and written in natural language.
`goal` is optional and describes the broader end goal you are ultimately trying to accomplish on behalf of the user. GitBook uses it to tailor the answer towards what is most useful for that goal.

The response will contain a direct answer to the question and relevant excerpts and sources from the documentation.

Use this mechanism when the answer is not explicitly present in the current page, you need clarification or additional context, or you want to retrieve related documentation sections.