> ## Documentation Index
> Fetch the complete documentation index at: https://docs.ntop.com/llms.txt
> Use this file to discover all available pages before exploring further.

# How to export your design to ANSYS Workbench

## Objective:

Learn how to export FE Data to ANSYS Workbench using different FE data options.

## Procedure:

There are different options to choose from while exporting FE data. Based on the requirement, you can choose the most appropriate option.

| **Block**                                                    | **Nodes** | **Elements** | **Materials** | **Element Sets** | **Node Sets** | **Boundary Conditions** | **Analysis Settings** |
| ------------------------------------------------------------ | --------- | ------------ | ------------- | ---------------- | ------------- | ----------------------- | --------------------- |
| [Export FE Mesh - no sets](#h-01fdamqaabmcsnpdjfchgyz4e1)    | **🗸**    | **🗸**       |               |                  |               |                         |                       |
| [Export FE Mesh - with sets](#h-01fdamqaabmcsnpdjfchgyz4e1)  | **🗸**    | **🗸**       |               |                  | **🗸**        |                         |                       |
| [Export FE Model - no sets](#h-01fdamqr737d23sw0mzeys512r)   | **🗸**    | **🗸**       | **🗸**        | **🗸**           |               |                         | **🗸**                |
| [Export FE Model - with sets](#h-01fdamqr737d23sw0mzeys512r) | **🗸**    | **🗸**       | **🗸**        | **🗸**           | **🗸**        |                         | **🗸**                |
| [Export Static Analysis](#h-01fdamr6jv36hv2pa17sn7m11f)      | **🗸**    | **🗸**       | **🗸**        | **🗸**           |               | **🗸**                  | **🗸**                |

##

## Exporting FE Mesh with Sets

1. Generate a [FE Mesh](https://support.ntopology.com/hc/en-us/articles/360037005234-How-to-create-an-FE-Volume-Mesh) for the model and [Boundary conditions](/help-articles/knowledge-base/structures/how-to-use-boundary-conditions).

2. Use the **Export FE Mesh** block.

* Input the Mesh and add the Boundaries in the sets field.
* Update the Path for Mesh Export.
* Select the file type as **Ansys Mechanical Input** **(.cdb)**

![A gif showing how FE Boundaries can be exported using the Sets input of the Export FE Mesh block.](https://files.learn.ntop.com/help-articles/interop/4402711116819.png)

![The FE Mesh with the boundaries highlighted. ](https://files.learn.ntop.com/help-articles/interop/4402706549651.png)

3. Import the exported **Ansys Mechanical Input** **(.cdb)** file into Ansys Workbench.

![Importing the External Model into Ansys Workbench.](https://files.learn.ntop.com/help-articles/interop/4405434951443.png)

4. Open **Setup** to modify properties in the Schematic for the External Model

* Select cell **2A** to expose the properties pane
* Uncheck **“Check Valid Blocked CDB File”**

**![The properties of the imported external model. The data source file name is highlighted, as well as the Check Valid Blocked CDB File option.](https://files.learn.ntop.com/help-articles/interop/4402706601491.png)**

5. Open the **Model** in Mechanical Model/Static Structural.

* Update it to see the Mesh and Sets are imported as**Named Selections.** The material for all elements is selected by default when importing a FE Mesh.

**![The FE Mesh with the boundaries highlighted in Ansys Workbench. ](https://files.learn.ntop.com/help-articles/interop/4402706617363.png)**

6. Apply Boundary Conditions to the Named Selections using **Direct FE** in the Environment Ribbon. Note that node sets only support boundary conditions in the **Direct FE** dropdown. Other boundary conditions are can be applied to geometry which Ansys detects from the mesh.

![The Direct FE options menu is highlighted. These Boundary Conditions can be applied to the imported boundary selections.](https://files.learn.ntop.com/help-articles/interop/4405398254995.png)

7. Solve the FE Setup and add plots you wish to visualize. See examples of this below: ![The top image shows the static analysis run in Ansys and the bottom image shows the same analysis run in nTop.](https://files.learn.ntop.com/help-articles/interop/4405401323667.png)

## Exporting FE Model with Sets

1. Generate [FE Model](/help-articles/knowledge-base/structures/how-to-create-a-simulation-model) and [Boundary Conditions](/help-articles/knowledge-base/structures/how-to-use-boundary-conditions)

2. Use the **Export FE Model** block

* Insert the **FE Model**
* Update the Unit system
* Add the boundaries in sets
* Select the file type as **Ansys Mechanical Input** **(.cdb)**

![An FE Model with specific boundaries highlighted.](https://files.learn.ntop.com/help-articles/interop/4402711262483.png)

3. Open the exported FE Model (.cdb) file in your preferred code editor.

* Scroll down to the bottom or find "**SOLUTION**".
* Comment out the last 4 APDL analysis commands by typing **C\*\*\*** before the command.

![The exported FE Model cdb file open in Notepad ++.](https://files.learn.ntop.com/help-articles/interop/4405448340499.png)

4. Import the FE Model (.cdb) file into Ansys Workbench.

* Double click **Setup** (this opens up the Outline for the Schematic for the External Model).
* Click Cell "\*\*C2"\*\*and uncheck the **“Check Valid Blocked CDB File”.**
* **Connect to Model and Engineering Data cells.**

![The External Model cdb file imported into Ansys Workbench, the file's properties panel is open.](https://files.learn.ntop.com/help-articles/interop/4405448475027.png)

![Importing the External Model into Ansys Workbench.](https://files.learn.ntop.com/help-articles/interop/4405457545619.png)

5. Apply **Direct FE** Loads and Restraints using the Named Sets.

* Refer to Step 7 in the instructions above.
* Solve the Static Structural Analysis on the FE Setup.

![A static structural analysis run in Ansys Workbench.](https://files.learn.ntop.com/help-articles/interop/4405450599827.png)

## Exporting a Static Analysis

1. Run Static Structural Analysis in nTop. You can find detailed instructions on FE Model Preparation, Generating Boundary Conditions, and applying Loads here [How to run a static analysis](/help-articles/knowledge-base/structures/how-to-run-a-static-analysis).

2. Use the **Export Static Analysis** block.

* Update the input fields with the necessary **FE Model**, Boundary Conditions, and Unit System.
* Select the file type as **Ansys Mechanical Input** **(.cdb)**

![An example of exporting a static analysis from nTop.](https://files.learn.ntop.com/help-articles/interop/4405462899987.png)

2. Open the exported **Static Analyis** (.cdb) file in your preferred code editor.

* Scroll down to the bottom or Find "**SOLUTION**".
* Comment out the last 4 APDL analysis commands by typing **C\*\*\*** before the command.

![The exported static analysis cdb file open in Notepad ++.](https://files.learn.ntop.com/help-articles/interop/4405463771027.png)

1. Import the **Static Analysis** (.cdb) file onto Ansys Workbench.

* Double click Setup (this opens up the Outline for the Schematic for the External Model).
* Click Cell "**C2**" and uncheck the **“Check Valid Blocked CDB File”**.
* Connect to Model and Engineering Data cells.
* Check Step 4 in the Export FE Model section for reference.

2. Update the Solution in the Static Structural Block to solve the FE Setup.

* Element sets come over in the Named Selection branch.
* There are node sets when importing a Static Analysis, unlike FE Mesh and Model.
* The material model is assigned to the element set.
* Boundary conditions can be viewed in its folder.

![The Static Analysis imported into Ansys Workbench.](https://files.learn.ntop.com/help-articles/interop/4405458134291.png)

And that's it! You've successfully learned to export FE Data to ANSYS Workbench.

Are you still having issues? Contact the [support team](https://support.ntopology.com/hc/en-us/requests/new), and we'll be happy to help!

## Download the Example file:

* [Example file](https://files.learn.ntop.com/Support%20Article%20Example%20Files/Knowledge%20Base/User%20Interface/Export%20to%20Ansys%20Workbench%20Example.ntop)

## Keywords:

*FE mesh export static analysis ansys model FEA ANSYS how-to workbench*