1Creation and Use of a Superlement in a Rotor Model

RD_TU_F_005
SAMCEF Rotors, Rotor analysis within SAMCEF Field tutorial :
Super-Element creation and use
Learning Objectives:
Introduction and familiarisation to FIELD and ROTOR : creation and use of superelement in a Rotor model.
Estimated time required: **mins Challenge level: Advanced
Document Reference:
Author : / RD_TU_F_005
Patrick Morelle
Date: / 16th February 2012

“I can‟t understand why people are frightened of new ideas. I’m frightened of old ones.” – John M. Cage Jr.

1Creation and use of a superlement in a rotor model

The objective of this tutorial is to analyze the critical speeds of the rotating assembly. In this example we create the geometry as a super element which is then used as such in a rotor model. The specific loading and constraints for this analysis are applied to the Super Element.

Fig. 1

2Perequisite

First go through tutorial RD_TU_F_004for a first critical speed analysis exercise involving Samcef FIELD and ROTOR and a 2D model.

3The topics covered in this exercise are :

How to define 2D rotor geometry in Field (vertex, lines, face)
How to define an elastic material
How to create a superelement from this 2D geometry
How to create a model, and import the superelement in it
How do define a Lumped mass attached to the superelement
How do define a Ground bearing linked to retained nodes of the superelement
How do define locking on translational degrees of freedomof the superelement
How to perform a “critical speed” analysis (ROTOR) of the model containing the superelement
How to examine the results and report them.
How to perform recovery of the superelement and see internal modal displacements

1Creation and use of a superlement in a rotor model

2Perequisite

3The topics covered in this exercise are :

4Methodology

5Establishment of simulation strategy

6Creating the super element

6.1Defining the model geometry

6.2Assign the Analysis data

6.3Mesh the model

6.4Run the calculations

6.5Import of a superelement

6.6Launch the calculations of the global model

6.7Examine the results

6.8Recover the results

Creation of a super element

4Methodology

The creation and use of a superlement based on “2D” models for rotor dynamicscorresponds to the following methodology :

Establish the strategy for the simulation of the rotor (idealization)
Start Samcef Field with the option “super element creation”
Create the geometry of the 2D model using the Field modeler
Associate analysis data to the previously created geometry
Mesh the model
Create the superelement (condensation)
Start Samcef Field with the option “critical speed analysis”
Create a rotor model based on the previously created superelement
Launch the analysis
Visualize the results
Perform recovery of the superelement so to see modal displacements

5Establishment of simulation strategy

In this tutorial you are going to idealize a rotating system (a “rotor”) using 2D “Fourier” elements. However, this model will be build in two phases :

1.We shall create the model geometry and associate proper material data. We shall then mesh the model and condensate it

6Creating the super element

Start SAMCEF Field software, and select “Rotor Dynamics” as the Domain of application :

Fig.2

2. Select “Super Element Creation” as the “Analysis Type”:

Fig.3

6.1Defining the model geometry

The active module of Field is for the moment, the “Modeler” one. This system will be modeled using a 2 D representation of the axi-symmetric section of the rotor. We shall first create the points/vertices of the 2D geometry. We will create the 2D surface in the XZ plane.

Click on the Create vertex tool .

In the Create Vertex dialog that appears (Fig. 7), keep the value X=Y=Z=0 mm, and click [Apply]

Fig. 4

Using the same “create vertex” dialogue box, you can now enter the coordinates of the other points we need (don’t forget to hit <Enter> after each new data and to click on [Apply] to really create them). Define the following points :

Point number / X Coordinate in mm / Z Coordinate in mm / Name
1 / 0 / 0
2 / 5.1 / 0
3 / 5.1 / 12.7
4 / 10.2 / 12.7
5 / 10.2 / 50.8
6 / 7.6 / 50.8
7 / 7.6 / 76.2
8 / 20.3 / 76.2
9 / 20.3 / 88.9 / Disk
10 / 20.3 / 101.6
11 / 33.0 / 101.6
12 / 33.0 / 106.7
13 / 33.0 / 114.3
14 / 25.4 / 114.3
15 / 25.4 / 127
16 / 25.4 / 134.6
17 / 12.7 / 134.6
18 / 12.7 / 165.1 / Bearing A
19 / 12.7 / 190.5
20 / 15.2 / 190.5
21 / 15.2 / 266.7
22 / 12.7 / 266.7
23 / 12.7 / 287.0 / Bearing B
24 / 12.7 / 304.8
25 / 38.1 / 304.8
26 / 38.1 / 315.0
27 / 20.3 / 315.0
28 / 20.3 / 345.5
29 / 20.3 / 355.0
30 / 15.2 / 355.0
31 / 15.2 / 345.4
32 / 0 / 345.4
33 / 0 / 127.0
34 / 17.8 / 127.0
35 / 17.8 / 114.3
36 / 15.2 / 114.3
37 / 15.2 / 106.7
38 / 0 / 106.7

The 38 points will appear in the Data tree and in the viewer. When it’s done, your graphic window looks like this :

Fig. 5

You are now going to create a wire linking those points. Click on the Create Wire tool . The following menu appears.

Fig. 6

First click on the “Closed line” option to make it active. Then, click on the first vertex. Then click on the second vertex. Then the third …. Until you close the wire and see what corresponds to this :

Fig. 7

Click [Apply] to create the wire.

Click on the button. It opens the following dialogue box :

Fig. 8

Select the wire and create the face based on it. You see the following :

Fig. 9

6. You can rename the face by selecting it in the data tree and selecting Edit - Rename from the menu bar. In this example the face has been renamed "Rotor-shaft". Now that the face has been defined, you can hide the wire and the points used to generate it. Select them in the data tree and select Hide from the pop-up menu.

The geometry of the super element is defined, we will now define the properties of the structure.

Save this first version of your model with the “Save” option, or with the “Save as” one. We shall give the name “RD5_1.sfield” to the model.

6.2Assign the Analysis data

Click on Analysis data .
With the face selected, click on Behavior . Select Volume Fourier. From the Placed on options select Face. You see the following :

Fig. 10

Click [Apply] so to create the behavior and you see a new symbol appearing in your Graphic Display :

Fig. 11

Select the face in the tree, right click on it and select Rotor from the pop up menu :

Fig. 12

A dialog will appear in which you can define the properties of the Rotor :

Fig. 13

Because we are not using a beam, it is necessary to define the axis of rotation which in this case is in the Z direction.Click [Apply] then [Close].

We shall now define the material characteristics. Again making sure that the model is selected, click on Material . Select the unit “MPa” for the Young Modulus value, then enter the value “205000”. You should always select the unit before you enter the value.Enter a value of “0.3” for Poisson Ratio. Enter a value of “7800” kg/m3 for the mass density. Click [Apply] then [Close] to finish defining the material properties. You see a new data “Elastic_on_1_face_of_Face1” appearing in your Data Tree :

Fig.14

Double clicking on it would re-open the dialogue box and allow you to check/correct/modify the defined data.

When creating a Super Element, you need to specify the particular nodes that will be retained allowing the Super Element to be connected to the “external world”. In this case we will retain the nodes where the disk and the bearings are supported. Select the face and click on the Constraint tool. Select Retained node from the Constraint options.

For Rotor dynamics we need to assign relate the nodes to a rotor. Select Center Node from the Choose options and then check the button next to Rotor.

From the Placed on options select Vertex then click on point 9 (where the disk will be located), points 18 and 23 (where the bearings are located). Click [Apply] each time to define the retained nodes. (Select Show from the contextual menu to help locate the correct vertices.)

Fig. 15

All the mechanical properties of the model have been defined. We can now mesh the Super Element.

6.3Mesh the model

Click on the Mesh Module . Apply as mesh constraint a length of “2” mm for the mesh, select “parabolic” as element type, then click on the Generate tool , click on [Apply] then [Close]. You get the following :

Fig. 16

6.4Run the calculations

Click on Solver .
Click on Convert and Launch . Depending on Samcef Field settings, the following warning message may appear :

Fig. 17

Close it and the following dialogue box opens :

Fig. 18

In the Files & Memory tab, check the paths and memory data. For a Super Element Creation it is recommended not to use a temporary directory as the Working Directory and to not to accept the default. That was the meaning of the warning message asking you in fact to select a directory where the super element files are going to be stored for further usage.

Click on the Creation Parameters tab. In this tab you can specify the frequency range and the modes to be determined for the super element. It is usual to specify an upper frequency value that is 2 times the normal maximum frequency range to which the super element will be submitted.

Select Dynamic as the Type of super element. Enter a value of 20 in the Number of Eigen Values field. Enter the value of 0Hz for the Minimum frequency field. Enter the value of 3600Hz for the Maximum frequency field.

Fig.19

Click on the [Advanced] button and select the Component Mode as Condensation Algorithm.

Click on the “Eigen Values and Sweeping” tab. You see now the following dialogue box :

Fig.20

Launch the analysis by clicking on. You obtain the following :

Fig. 21