> 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/create-stress-model-input-file-by-editing-thermal-model-input-file.md).

# Create Stress Model Input File by Editing Thermal Model Input File

## Change the heading name (optional)

```
*Heading 
** Job name: Cylinder_2D_s Model name: Cylinder_2D_s
```

## Change the element type from thermal element to stress element

```
*Element, type=DCAX4
```

* to

```
*Element, type=CAX4
```

## In the ***\*Step*** definition for all the steps, change ***\*Heat Transfer*** to ***\*Static***

<figure><img src="https://3062023715-files.gitbook.io/~/files/v0/b/gitbook-x-prod.appspot.com/o/spaces%2F0UQEr9tolIKQwZXdPc9a%2Fuploads%2FS1sBgk7wsVw7gkxVBCr1%2Fimage.png?alt=media&amp;token=dbb0df55-d522-4e72-9631-efa898b82abc" alt=""><figcaption></figcaption></figure>

## Fix one node for the stress analysis

***Inside Assembly***

```
*Nset, nset=Fixed_Y_Node, instance=cylinder-2d-1
16,
```

**After Assembly, and before \*Step**

```
*BOUNDARY
Fixed_Y_Node, 2, 2
```

## Change the ***User Material type***&#x20;

from ***Thermal*** to ***Mechanical,*** and change the second material constant from -3 to -4.

```
*User Material, constants=24, type=THERMAL
** Row1 (1rd:Density),(2nd:ModelType),(3rd-8th:F,P,UB,LB,M,TM)
7.83e-06,    -3.,    0.3,    0.7,     0.,     0.,     0.,     0.
** Note: with "-1.", the default alloy value from the material database will be used
** The default value is available in material *DQT file or the Powepoint pdf file 
** Row-2: GS:1, Mn:3, Si:4, Ni:5, Cr:6, Mo:7, Cu:8,  V:9
        0.0635,  0.6,  0.3,  0.1,  0.1, 0.05,  -1.,  -1.
** Row-3: P:10, Nb:11, Al:12, Ti:13,  W:14, Co:15,  B:16,  N:17  
           -1.,   -1.,    0.,    0.,   -1.,   -1.,    0.,   -1.
```

to

```
*User Material, constants=24, type=MECHNICAL
7.83e-06,    -4.,    0.3,    0.7,     0.,     0.,     0.,     0.
0.0635,    0.6,    0.3,    0.1,    0.1,   0.05,    -1.,    -1.
-1.,    -1.,     0.,     0.,    -1.,    -1.,     0.,    -1.
```

## Define ***\*Controls*** card in the first step.

```
*CONTROLS, PARAMETERS=LINE SEARCH
6,
*CONTROLS, PARAMETERS=TIME INCREMENTATION
20, 30
*CONTROLS, FIELD=DISPLACEMENT, PARAMETERS=FIELD
0.05, 0.05,
```

## Define ***\*Output*** card for displacement, stress, and SDV.

```
*Output, field, frequency=10
*Node Output
NT, U
*Element Output
S, SDV1,SDV2,SDV4,SDV21,SDV34,SDV47,SDV60,SDV73,SDV86,SDV99,
SDV102,SDV103,SDV104,SDV105,SDV106,SDV107,SDV108,SDV115,SDV117,SDV135,
SDV142,SDV149,SDV156,SDV157,SDV172
```

## Change ***\*Sfilm*** definition to \*&#x54;***emperature file*** input for all the steps

```
*Sfilm, OP=NEW
Outer_Surface, ...etc
```

to

```
*TEMPERATURE, FILE=thermal, BSTEP=1, ESTEP=1
```

## Modify the output including the ***monitor DOF***

```
*Monitor, DOF=1, node=A_Monitor_Node, frequency=1
```

## **Start the simulation using the following command**

```
abaqus job=cylinder_2d_s
```