Taking Advantage of Symmetry in CATIA V5 GPS
Patrick Pagtakhan, P.Eng., Mecanica Solutions Inc.
1. Introduction
This article details how to take advantage of symmetry for the purpose of carrying out a simple static analysis. With the use of a mechanical mounting piece, we will demonstrate a specific case in which the design is symmetric in shape and subjected to symmetric loading conditions.
2. Example of a mechanical mounting piece
In Figure 1, a central mounting piece is subject to a large temperature change and is press-fit into 8 radial components. We want to determine if this thermal cycling will be an issue in the design, so it is important to find out the stress level in the model.
Figure 1: Mounting piece
2. Full Model Analysis
We will solve this problem without symmetry and then taking advantage of symmetry.
In Figure 2, we applied a temperature field of 573.15K to the mounting piece, which was initially at an environmental temperature of 293.15K. The inside of all eight arcs are clamped to simulate a simple press-fit with no initial compression.
Figure 2: Thermal and mechanical loading
Figure 3 shows the first look at the analysis:
Figure 3: Analysis display
Closer inspection shows that at an element setting in size 10mm and parabolic results in Global Estimated Error Rate of 6.02924%. (Figure 4)
Figure 4: Analysis results
Inspecting the Von Mises Stress Fringe closely shows that the global maximum and nodes in similar positions throughout the mesh are close to this % error.
Figure 5: Detailed area of maximum stress
The global maximum is estimated to be 1.796 E9 N/m^2 and a sample node point in a similar geometrical location on the model is approximately 1.66 E9 N/m^2. To obtain better results, a finer mesh could be applied, which would increase computational time.
3. Using Symmetry
In order to take advantage of symmetry, the model geometry and the boundary conditions must be symmetric. In this case both criteria are satisfied, which allows us to proceed to cutting the model in its symmetric planes. Figure 6 shows that only 1/16th of the entire model is required in order to exploit the symmetry relative to the center point.
Figure 6: Symmetry of mounting piece (1/16th model)
Once the model has been divided up, local axis should be created to handle the symmetry boundary conditions. Figure 7 shows the two axis systems on the piece of the model.
Figure 7: Symmetric model of mounting piece
The original boundary conditions can then be re-applied in the GPS module of CATIA V5. Figure 8 shows the clamp restraint on the inside of the arc and the temperature field applied.
Figure 8: Thermal and mechanical loading
Use the  icon to apply the symmetric constraints. On the model, choose the face which is the mirroring plane. Then, under "Axis System" in the "Type" window scroll down to "User", turn on the radio button for "Display locally" and choose the axis system that corresponds to the mirroring plane. Following these steps will facilitate the visualization of the required degrees of freedom. Figure 9 illustrates the view you should see up to this point.
Figure 9: Symmetric constraints
To satisfy the laws of symmetry, the geometry cannot cross over the highlighted symmetry plane shown in Figure 9. However, the geometry can "slide" in that plane.
The best analogy would be to imagine half a grapefruit on a mirror, you can slide it in the plane of the mirror, but if you try to rotate it into the mirror or lift it off, you get grapefruit juice or you break the reflection.
The Restrain list, as shown in Figure 9, must demonstrate the following restraints:
Free to slide along Axis 1 (X direction) therefore Restrain Translation 1 should be unselected.
- Cannot move along Axis 2 (Y direction), it would be crossing the mirroring plane or lifting off the mirroring plane, therefore Restrain Translation 2 should be selected.
- Free to slide along Axis 3 (Z direction) therefore Restrain Translation 3 should be unselected.
- Cannot rotate about Axis 1 (X direction), it would be crossing the mirroring plane or lifting off the mirroring plane, therefore Restrain Rotation 1 should be selected.
- Can rotate about Axis 2 (Y direction), therefore Restrain Rotation 2 should be unselected
- Cannot rotate about Axis 3 (Z direction), it would be crossing the mirroring plane or lifting off the mirroring plane, therefore Restrain Rotation 3 should be selected.
Figure 10 illustrates the restraint selection.
Figure 10: Restraint setting
The symmetry constraints can then be applied to the other mirroring plane following the same procedure with the final result illustrated in Figure 11.
Figure 11: Analysis display
This analysis had a much lower global error and ran much faster than the full model. In addition, the element size was much smaller, thus allowing a smoother fringe plot.
4. Conclusion
It should be noted that the key benefit to utilizing symmetry is that the solve time will be greatly reduced versus using a full model. In addition, refining the mesh and re-running the analysis will also be less time consuming.
The main limitation of this method would be in the calculation of natural frequency. In the case of symmetry constraints on a frequency analysis, only the symmetric modes will be found.
Company Drawing Standards Applied Using Generative View Styles in CATIA V5
Eric Hildebrand, MSC.Software Corporation
Why would I use a Generative View Style?
The way in which a view appears in a CATIA V5 drawing can be different for each view. One view might show hidden lines while another does not. One view might display fillet boundaries while another might display just the projected edges of the fillets. These types of view display properties can be modified for each view individually. While this provides a great deal of flexibility, it may result in views that do not conform to the acceptable drawing standards of your company.
An efficient way to produce views that meet standard display criteria is to use Generative View Styles. A company standard combination of view display properties can be saved as a Generative View Style. This custom Generative View Style can then be applied to one or more views in the drawing, ensuring that the view complies with acceptable company standards. Each view can have a different Generative View Style applied to it. See examples in Figure 1.
Figure 1: Example of two different view styles
Creating a custom Generative View Style
There are a number of generative standard files already provided by Dassault with V5. As a CATIA user, you have access only to view these standards by selecting "Tools + Standards", then choosing "generativeparameters" as the category in the Standard Definition window. By selecting the drop down arrow next to the File field, you can display the standard files (Figure 2).
Figure 2: Dassault provided generative standard files
The first selection in the list is the default Generative View Style - appropriately named "DefaultGenerativeStyle.xml". To see the detailed content of the properties defined in the standard, click on a gray node with a plus sign in the left column of the window. The tree will be expanded. The value for the highlighted item is displayed in the right column (Figure 3). Notice the value is displayed but the field is grayed out. A user does not have the ability to modify this value.
Figure 3: Tree expanded to display value for highlighted item
A custom Generative View Style can be created when running V5 in administrator mode. The standards are accessed in the same manner by selecting "Tools + Standards", choosing "generativeparameters" and selecting the file "DefaultGenerativeStyle.xml". Values in the right column of the Standard Definition window can now be modified. For example, to activate the display of hidden lines, expand the tree and select the Hidden Lines item (Figure 4). Change the value from "No" to "Yes" in the value field using the drop down arrow (Figure 4). Setting the standard to "Yes" means that hidden lines will be displayed in the view.
Figure 4: Modifying the display for hidden lines in a Generative View Style
After making all of your changes in the standards, click on the "Save As New" button at the bottom of the Standard Definition window. Now specify a name for the new Generative View Style and save it in a directory created to store your company standard files. This directory should be specified by the CATCollectionStandard variable in the V5 Environment Editor. The custom Generative View Style you just created will now be available from the list of standard files (Figure 5).
Figure 5: Custom Generative View Style has been created
Applying a custom Generative View Style to a view
To allow the use of Generative View Styles, first de-select the option to prevent their use.
Access "Tools + Options", and under "Mechanical Design" select the "Drafting" branch. Select the "Administration" tab, and under the "Generative view style" section, de-select the option "Prevent generative view style creation" (Figure 6).
Figure 6: De-select the option preventing the use of Generative View Styles
When creating a new view, the view style selection window appears. Choose the custom view style from the drop down arrow (Figure 7). Continue with the creation of the view.
Figure 7: Select the custom view style when creating a new view
To apply the custom view style to an existing view, point to the view frame using your cursor and click the right mouse button. Select the option "Set View Style" from the view object menu under "Generative View Style" (Figure 8). Choose the custom view style from the list of standards displayed in the window (Figure 9) then click OK. Update the view to see the view style applied.
Figure 8: Select the option to apply a view style
Figure 9: Select the custom view style to be applied
To copy the view style from one view onto another view, point to the view frame of the sending view and click the right mouse button. Now select the option "Apply View Style To" from the view object menu under "Generative View Style" (Figure 10). Select the frame of the view that the custom view style will be applied to. Update the view to see the view style applied.
Figure 10: Select the option to copy a view style to another view
After you have created custom Generative View Styles that meet the needs of your company's drawing standards, V5 users should be encouraged to only create drafting views using the company Generative View Styles. This will allow drawing views to be generated quickly and ensure that each view complies with acceptable company standards.
Using iXFelec - XML Files to Place Electrical Devices
Nicolas Grise, Dassault Systemes
Introduction
In today's context of full 3D product definition, electrical systems pose a complex modeling challenge. This is mostly due to two factors:
- The variety of shapes, parts and relationships necessary to obtain an accurate 3D DMU of electrical systems
- The need to drive modeling by upstream requirements and to drive downstream documentation.
This first article will cover the basic functionality and workings of CATIA V5 specification-driven electrical part placement capabilities. Further articles will expose functionality and environment setup in more detail.
| Definitions |
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| CATIA V5 Catalog: |
CATIA Document used to classify components in families and chapters. A component is a reference to an external document or an entity such as a feature (e.g. PowerCopy), V4 documents (e.g. models) or V5 documents (e.g. CATPart, CATProduct, etc.) described with keyword values.
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| XML / iXFElec File: |
File generated manually or programmatically in Dassault Systèmes' IXF format using XML language. The file contains the electrical devices and their internal relationships within a wire harness (i.e. Connectors, contacts, wires, splices, equipment …).
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Electrical Device
Type: |
CATIA V5 Attribute assigned to a CATPart of CATProduct identifying it as a specific type of electrical part in CATIA and providing the part with behaviors allowing the user to define electrical connection points and properties. (Ex.: "Single Insert Connector" is the Electrical Device Type that is assigned to CATPart representing a plug-type connector.). |
Functionality
The CATIA V5 functions used to perform Specification-Driven Part Placement are found in the Electrical Assembly Design Workbench of the Equipment & Systems Solution.
 Select External Systems
 Manage Links
Principles-relationships (through example)
In order to illustrate the fore mentioned functionality, let us consider the scenario where an upstream requirement dictates that a specific connector be a part of a specific electrical wire harness.
We will first explore the different documents involved: The connector, the catalog and the xml file. Secondly, we will see how these documents work together to perform the scenario.
The connector
Let the connector part number be PN_SIC1234 and let the connector's unique identifier within the harness be ID_SIC1234. The connector PN_SIC1234 is modeled as a CATIA V5 CATPart and is assigned the "Single Insert Connector" Device Type. The connector PN_SIC1234 is stored in a catalog.
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Part Number = PN_SIC1234
Identifier = ID_SIC1234
Electrical Device Type = Single Insert Connector
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Connector Example
The catalog
The catalog document contains pointers to other documents and organizes them in a logical fashion, much like a book's table of content. In this case, a family named "Single Insert Connectors" houses a link to the connector PN_SIC1234 used in this example.
Catalog Example
The xml file
The upstream information is fed to CATIA V5 through an xml file. The file is used to list the electrical components in the wire harness and contains information about the components. Information about the connector used in this example is listed as follows:
- Identifier: id = "ID_SIC1234"
- Device Type: xsi:type = "tns:Connector"
- Part Number: <NS1:PartNumber>PN_SIC1234</NS1:PartNumber
xml File Example
Integration
These 3 documents are used together to drive the harness 3D definition. The relationship between them is managed by CATIA V5 through various option settings, mainly "Electrical Mapping": and "Electrical Process Interfacing".
"Electrical Mapping" maps the CATIA V5 Electrical Device Type to the Catalog family containing parts of that type. Here, we are indicating that the Catalog family "Single Insert Connectors" contains parts that have the "Single Insert Connector" Electrical Device Type.
"Electrical Process Interfacing" specifies the location of the xml file.
Electrical Mapping Example
Electrical Process Interfacing Example
1. Starting with a CATProduct and using the "Select External Systems" function, we set our xml file as the "Current System". Typically, one xml file lists all the devices for one harness.
2. Using the "Manage Links" function, we see the xml file's content. The "Place" button queries the catalog using both the Part Number and the Electrical Mapping. Once the query is validated, the component is instantiated in the wire harness CATProduct and assigned the identifier's value to the Instance Name and the Reference Designator parameters of the connector.
Conclusion
We have seen the basic electrical part placement capabilities of the CATIA V5 Equipment & Systems Tools. The principles seen here apply to many other electrical devices that cover a broad range of electrical modeling scenarios.
Further detail on electrical integration and setup guidelines will follow in future articles.
Nicolas Grisé
CATIA V5 Consultant
Dassault Systemes Inc.
(206) 612-2954
nicolas_grise@ds-ca.com
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