# The ABAQUS FAQ

## Q7.1 : How do I apply point loads?

Use the following statements for example. The data lines after the keyword line *CLOAD contain the Node number and the Components of loads in the X, Y and Z directions respectively. One dataline per node.
```*CLOAD
100,  0., -100., 0.
101,  0.,  -80., 0.
```

If the same load is to be applied to a number of nodes then these nodes can be made into a set and single data line could be used as follows :
The nodes listed are grouped together in a set called NDLSTA.
```*NSET,NSET=NDLSTA
100, 110, 120, 130, 140
.....

NDLSTA,  0., -100., 0.
```

If using ABAQUS/CAE select module Load and click on the Create load icon. In the new form select Concentrated force and click on Continue....
In the viewport area click on Points to be applied the Forces and then click on Done. Hold down the SHIFT key to make multiple selections. Hold down the CTRL key to de-select any points previously selected.
In the dialogue box which pops up enter the load in the box for the appropriate directions, CF1, CF2 and CF3 are for X, Y and Z directions respectively. Click on OK to complete the process.

## Q7.2 : Is it possible to apply point loads w.r.t. to local co-ordinates?

Yes it is possible to apply point loads w.r.t to local co-ordinates.

Consider the figure where nodes 1 to 5 along the outer radius are to be subjected to a radial outward force of 1 unit. A local cylindrical co-ordinate system transformation is set up first. The nodes 1 to 5 are grouped into an element set called CID1. The transform keyword is used to apply the transformation to the node set CID1 as follows :
```*TRANSFORM, TYPE=C, NSET=CID1
0.,          0.,          0.,          0.,          0.,          1.
**
*NSET, NSET=CID1
1,       2,       3,       4,       5
**
**
**
1, 1,          1.
2, 1,          1.
3, 1,          1.
4, 1,          1.
5, 1,          1.
```

The applied loads are interpreted according to the transformation.

If using ABAQUS/CAE folow select the Load module. Click on the Create Datum CSYS co-ordinate system. Choose the appropriate icon from the collection of icons. In the dialogue box which pops up select the required co-ordinate system out of the choice offered : Rectangular, cylindrical and spherical.
Then click on continue. Answer the questions posed in the prompt area and enter any values prompted for. Then click on the Red cross to complete the process.
In the new form select Concentrated force and click on Continue....
In the viewport area click on Points to be applied the Forces and then click on Done. Hold down the SHIFT key to make multiple selections. Hold down the CTRL key to de-select any points previously selected.
Click on the Edit button next to the Global CSYS entry and in the prompt area click on Datum CSYS List and this will list the previously created co-ordinate system. Make the selection. Click on OK.
In the dialogue which pops up enter the load in the box for the appropriate directions, CF1, CF2 and CF3 represent the X, Y and Z directions respectively. Click on OK to complete the process.

## Q7.3 : How do I apply a uniformly distributed load?

Use the following lines of input to define a distributed load. Here 2D solid elements are used for this example.
```*DLOAD
40, P3, 50.  (Element 40 Side 3 is subjected to 50 units of loading)
TOP, P3, 10.  (Side 3 of all elements in set TOP is subjected to 10 units of loading)
```
```*DLOAD
SHLGB, P, 100.
```
Here the shell elements in element set SHLGB are subjected to 100 units of pressure loading in the direction of the positive normal to the shell. To apply the loading in the opposite direction make the load magnitude negative.

In the viewport area click on lines/edges (In 2D analysis) to be subjected to pressure and then click on Done. Hold down the SHIFT key to make multiple selections. Hold down the CTRL key to de-select any points previously selected.

In the dialogue box which pops up enter the load in the box marked Magnitude.
If the loading is Uniform leave distribution at the default setting. For Hydro-static or User definedclick on the down arrow after and make the selection.
For distribution click on Create and using the Create Expression Field and create an expression as a function of X and Y (for 2 Dimensional analysis). Then click OK.

## Q7.4 : How do I apply a non-uniformly distributed normal load?

Use the user subroutine DLOAD to specify a non-uniformly distributed load. See section 25.2.5 of the ABAQUS User's manual (Version 6.5).
This is illustrated for ABAQUS/Standard with a single C3D20R element where two vertical sides are subjected to normal pressure increasing lineraly with depth.
Input File (solid2.inp)

Analysis is submitted from the command line using the command :
This is also illustrated for ABAQUS/Explicit with a single C3D8R element where two vertical sides are subjected to normal pressure which is increasing lineraly with depth.
Input File (soliden.inp)

Analysis is submitted from the command line using the command :

## Q7.5 : How do I apply a varying shear load?

See the answer to the questions 7.18 and 7.19 below.

First the elements subjected to the gravity loading are grouped together in an element set. Then use the following statements. Also the density should be specified as part of the *MATERIAL record and then these properties assigned to the above element set.
```*MATERIAL, NAME=STEEL
**
*ELASTIC, TYPE=ISO
3.E+7,     0.3
**
*DENSITY
7800.

PLATE, GRAV, 9.8, 0.0, 0.0, -1.0
```
Here PLATE is the element set subjected to gravity loading which is defined by GRAV. For earth's gravity 9.8 is the actual magnitude. This is followed by the components of the gravity vector in X, Y and Z directions respectively. Here gravity acts in the negative Z direction.
For the axisymmetric case only the component 2 should be non-zero (-1).

If using ABAQUS/CAE select module Load and click on the Create load icon. In the new form select Gravity and click on Continue....
In the viewport area click on the region to be applied the Gravity and then click on Done. Hold down the SHIFT key to make multiple selections. Hold down the CTRL key to de-select any regions previously selected.
In the dialogue which pops up enter the load in the box for the appropriate directions, Component 1 2 and 3 represent X, Y and Z directions respectively. Click on OK to complete the process.
If the amplitude of the loading is not the default Ramp then click on create and choose the appropriate amplitude from the selection available and click on OK.

Define the element set to be subjected to the centrifugal loading. The magnitude is calculated as density multiplied by the square of the angular velocity (in radians/second). For axisymmetric problems the axis of rotation must be the global Z-axis, which must be specified as 0.0, 0.0, 0.0, 0.0, 1.0, 0.0.
```*DLOAD
PLATE, CENT, 225., 0.0, 0.0, 0.0, 0.0, 1.0, 0.0
```

The value of 225 is arrived at from a density value of 9 multiplied by the square of the angular velocity of 5 radians/sec.

If using ABAQUS/CAE select module Load and click on the Create load icon. In the new form select Rotational Body force and click on Continue....
In the viewport area click on the region to be subjected to the Centrifugal force and then click on Done. ABAQUS/CAE will prompt for 2 points to define the axis of rotation.
In the dialogue box select the toggle switch for Centrifugal for ther Load effect . Enter the value for Angular velocity and click on OK.
If the amplitude of the loading is not the default Ramp then click on create and choose the appropriate amplitude from the selection available and click on OK.

## Q7.8 : How do I apply a thermal loading ie heat input?

Section 19.4.4 of the users manual (Vol. V) gives an overview of the type thermal loading that can be applied.
1. Concentrated heat flux prescribed at nodes (*CFLUX)
2. Distributed heat flux prescribed at element faces (*DFLUX)
3. Body heat flux per unit volume (*DFLUX)
4. Boundary convection defined on element faces (*FILM)

### *CFLUX

```*CFLUX
56,  11, 10.
57,  11, 10.
```

Nodes 56 and 57 are applied a heat flux of 10 units. The number 11 represents the temperature d.o.f.

### *DFLUX

```*DFLUX
100, SPOS,  10.
```

A uniform surface flux of 10.0 per unit area is applied to the top face (SPOS) of element 100 which is a general heat transfer shell element.

### *FILM

Prescribing boundary convection :
Heat flux on a surface due to convection is governed by :

### Example

A uniform, time-dependent film condition can be defined for face 2 of element 3 by :
```*AMPLITUDE, NAME=sink
0.0, 0.5, 1.0, 0.9
*AMPLITUDE, NAME=famp
0.0, 1.0, 1.0, 22.0
...
**
*STEP
*HEAT TRANSFER
...
*FILM, AMPLITUDE=sink, FILM AMPLITUDE=famp
3, F2, 90.0, 2.0
```

A uniform, temperature-dependent film coefficient and a time-dependent sink temperature can be defined for face 2 of element 3 by
```*AMPLITUDE, NAME=sink
0.0, 0.5, 1.0, 0.9
*FILM PROPRETY, NAME=filmp
2.0,  80.0
2.3,  90.0
8.5, 180.0
...
**
*STEP
*HEAT TRANSFER
...
*FILM, AMPLITUDE=sink
3, F2, 90.0, filmp
```

### General

In the element type section in the ABAQUS user's manual the type of loading that can be applied is listed under each element type category. This type of loading is only applicable to the following element types :
1. Heat transfer elements
2. Coupled thermal-electrical elements
3. Coupled temperature-displacement elements

These categories of elements can be found under the following broader group of element types :
1. 1-D Solids (Only heat transfer elements are available)
2. 2-D Solids
3. 3-D Solids
4. Axisymmetric Solids
5. Shell Elements
Look for the heading Distributed heat fluxes under the element group and these list the type of heat input that can be specified.

### 2-D and 3-D Solids

• BF - Heat body flux per unit volume
• Sn - Heat surface flux per unit area into face n
Add NU after the load type if the heat input is non-uniform.

### Shell Elements

• BF - Heat body flux per unit volume
• SNEG - Heat surface flux per unit area into the bottom face of the element.
• SPOS - Heat surface flux per unit area into the top face of the element.
Add NU after the load type if the heat input is non-uniform.

For an analysis which consists of solely general steps the loads are considered to be total. For a perturbation step the load specified is treated as incremental ie ABAQUS will seek a response to the specified load about the base state. Here the base state is the state at the end of the last general step.

The output (displacements, stresses) will reflect this interpretation. These (displacements, stresses) are calculated as changes from the base state.

## Q7.10 : How do I remove the loading applied in a previous step?

This is illustrated with the *CLOAD type of loading. Specify with the option OP=NEW without any data lines.
```*CLOAD,OP=NEW
```

In a simple linear elastic static analysis all that is needed is the load magnitude. But in a more complex analysis - dynamics or nonlinear analysis it might be necessary to define loading that varies with time. One way ABAQUS allows for this is by using the *AMPLITUDE option (User's manual section 19.1.2, Vo. II, version 5.7).

Here the time and the load scale factors are listed in pairs. For example :
```*AMPLITUDE, NAME=UPDOWN
0., 0., 3.0, 1., 6.0, 1., 10., 0.
....
....
**
** step 1
**
*STEP,INC=50
*STATIC
0.1,5.0,
TOP, P3, 1000.
*END STEP
**
** step 2
**
*STEP,INC=50
*STATIC
0.1,5.0,
TOP, P3, 1000.
*END STEP
```

This first defines a time variation which rises linearly from a value of 0.0 at time zero to 1.0 at a time 3.0, remains at that value until a time of 6.0, then ramps down to 0.0 at a time of 10.0 as shown in figure.

This time variation is called UPDOWN, and is referred to on a *DLOAD option, where it governs the behaviour of a pressure load applied on side 1 (load type P1) of a set of elements called TOP. This magnitude will vary through time according to the amplitude definition, so that, for example, at a time 1.5 the pressure will be 500. The magnitudes specified in the AMPLITUDE option are used as scaling factors.
You will notice that because of the absence of the perturbation option in the *STEP keyword this is a general analysis where time accumulates. Because the step time is only 5.0 the loading of 1000 is applied and the unloading phase has not begun. In the second step which is also of duration of 5.0 units of time in the first 1.0 unit of time the loading remains unchanged. Then the loading is gradually reduced and at the end of the step it has reached the unloaded stage.
From the above example it should be clear that the *AMPLITUDE specification if necessary can span across more than one step in a general analysis.
If you are using the *AMPLITUDE option in a perturbation step then the time range cannot straddle more than one step. However it is perfectly acceptable to use *AMPLITUDE when the time used is the step time. The example below shows such a step. The amplitude definition UPDOWN remains unchanged. The following step has a step time of 10 units which is the same as the time range specified in the amplitude definition.
```**
** step 1
**
*STEP,PERTURBATION,INC=100
*STATIC
0.1,10.0,
TOP, P3, 1000.
*END STEP
```

## Q7.11 : What do I do to maintain the load at the same level as in a previous step?

Either re-specify the data input for the previous step or completely omit the load data input. If the loading was specified using *CLOAD keyword then omit these.

## Q7.12 : How do I change part of the previously applied loading?

```*CLOAD, OP=MODIFY
25, 0., -25.
```

Then the loading is modified for the listed nodes ONLY. At all other nodes the loading applied in the previous step using the *CLOAD keyword (for this example) remains unchanged.
```*CLOAD, OP=MODIFY
25, 0., -10.
```

Here the load level is reduced from -25 to -10. Notice that these are TOTAL loads. Here the minus sign only specifies the direction. One only considers the MAGNITUDE of the loading which always refers to the TOTAL load. With ABAQUS one always specify the total value of the load and NOT the incremental load.

## Q7.13 : How do I remove a single load which forms of group of loading which has already been applied in a previous step?

In the step in which you want to remove the single load re-specify the group of loading except for the load to be removed with the OP=NEW option. Here it is assumed that the type of loading is the same for the whole group (example : *CLOAD).
```....
**
25,  0., -25.
50,  0., -25.
75,  0., -25.
100,  0., -25.
....
** step in which the load applied to node 25 is removed
50,  0., -25.
75,  0., -25.
100,  0., -25.
```

## Q7.14 : Is it possible to specify a line load along a line of nodes?

This is only possible along a line element and not for a row of nodes along the edges of 2-Dimensional or 3-Dimensional elements.
In Load module click on Load Create button. In the dialog box select Traction and click on Continue... button. In the dialog box with the list of Types of loads select Line Load. Select Mesh and then click on the line element when prompted for Select Bodies for Load. Click on Done and then enter the magnitude of the loading in the boxes marked Component 1, Component 2 and Component 3. For Distribution select Uniform for uniform loading and User defined for non-uniform loading which would require writing a user subroutine called UTRACLOAD.

RAMP and STEP define how and when the loading is applied during a given step. The following figure shows the difference between the two.

Which of these two forms the default option depends on the procedure used for the step and the type of loading. See section 10.1.1 of the ABAQUS User's manual (version 5.5) for further explanation.

## Q7.16 : How do I apply a pressure loading to a shell element (S8R5) which is in the global X direction?

Use the following statements.
```*DLOAD
SHELL, BX, pressure-per-unit-thickness
```
SHELL is an element set consisting of all the shell elements subjected to pressure. The loading should be specified as a body force. Therefore divide the pressure by the thickness of the shell elements.

+

## Q7.17 : How do I specify a moving pressure loading (For example a wheel load of a vehicle)?

For this the subroutine DLOAD is required and this is illustrated with the following example.
A description which is also included in the subroutine
Input File (J15a.inp)