Links in CATIA
Julie Cyrenne, Dassault Systemes
Introduction
This article is the first of a series on the CATIA links. In this article, links are introduced and illustrated with the example of the design of a table. At each step of the design process, a link type is presented. The Five link types presented are the CCP link, the KWE link, the Instance link, the assembly constraint and the ViewLink.
Links Definition
A link is a dependency relation used to transmit geometric, parametric or positioning information between components. Links in CATIA are unidirectional and always point from the child to the parent. In other words, a child always knows what its parents are because this information is required to define its content. However, a parent doesn’t know whether it has children, because children have no impact on the definition of the parent. This architecture allows for the re-use of parents in different context.
The update of a part only updates the content of the part itself (and not the elements copied from external files). To ensure that all modifications to the external files are reflected in the part, check the option  in Tools/ Options/ Part Infrastructure/ General.
The Edit/ Links menu provides a list of all the external links of the part, if any, as well as the name and path of the pointed document and the status of the link.
Types of Links
Five types of links will be presented with the example of the design of a table: the CCP link, the KWE link, the Instance link, the constraint and the ViewLink.
The first CATPart contains the geometrical definition of the raw material used to create the table leg. The second CATPart contains the geometrical definition of the finished table leg. Consistency must be ensured between the models: a modification of the raw material must be reflected in the finished leg. For that purpose, the raw material part geometry is copied and pasted in the finished part (with the link maintained), where the machining operations are performed. Because the raw material and the finished leg will never be assembled together, this operation is performed outside the context of an assembly.
In this process, the raw material part is the parent: its definition is independent and is not affected by any modifications of the finished table leg. Therefore, no external links are created in the raw material part. On the other hand, the finished table leg is the child. Its geometrical definition is driven by the raw material part and will be affected by any modification of its geometry. This relation is represented by a CCP link in the finished table leg that points to the raw material.
The type of paste used is important in this operation. The figure below illustrates the three possible behaviors.
1/ If features are pasted using the regular paste or the paste special ‘as specified in the part document’, all the features are copied and no link is maintained to the source file.
2/ If features are pasted using the paste special ‘as result with link’, the geometry is copied (and not the features) and the link is maintained to the source file. This is the only type of copy that will create the CCP link.
3/ If features are pasted using the paste special ‘as result’, the geometry is copied (and not the features) and no link is maintained to the source file.
The CCP link is created in a part where geometry is pasted using the ‘Paste special as result with link’ functionality if the copy/paste operation is performed from part to part and outside the context of a product.
The leg socket is the common interface between the table leg and the tabletop. The dimensions of the socket are stored in parameters in the tabletop part. For the table leg to match the tabletop, those dimensions must match. For that purpose, the dimension can be copied (with the link maintained) from the tabletop to the table leg.
This link is in all points identical to the CCP link, except that parameters are copied instead of geometry.
| The KWE link is created in a part where parameters are pasted using the ‘Paste special as result with link’ functionality. |
To create a table assembly, the tabletop and table leg components must be inserted in the table assembly CATProduct.
In this process, the table assembly is the parent and the tabletop and table legs are the children. In the table assembly, an instance link is created for each component. This link carries the name and path of the files.
| The Instance link is created in a CATProduct where CATParts or CATProducts are inserted. |
Assembly constraints are used to position the parts of the assembly. Each leg will require an axis-to-axis coincidence and a surface-to-surface contact constraints to position it. 
The assembly constraints allow to position parts and products in the context of an assembly. This type of link cannot be visualized in the Edit/ Links menu. The links are stored in the CATProduct and apply to the instance of the components. In other words, an assembly constraint applies to a specific representation of a part in a specific assembly. For example, if the Leg.1 instance is constrained, all the other table leg instances are still free.
If the table leg style A was replaced by a table leg style B in the table assembly, all the constraints would be broken. The use of publications prevents this behavior. If the same publication name (Leg_Axis) is applied to both table legs’ axis, the assembly constraint will be reconnected automatically when the table leg is replaced with the second one. Publication is a topic that will be detailed in a future article.
| The constraint is created between two part/ product instances. The use of publications will allow to reconnect the constraints automatically when parts are replaced. |
The table leg CATPart contains the 3D geometrical definition and a CATDrawing contains the associated 2D representation. The views are generated from the CATPart using Generative Drafting functionalities. Whenever the part is modified, the drawing views indicate an update is required to reflect the changes.
This process does not create any external link in the CATPart (the parent). In the CATDrawing (the child), a ViewLink points to the CATPart (the parent). The ViewLink link is created for each generative view of a drawing. The information carried by the link is the name and path of the source model used for the projection.
| The ViewLink is created between in the CATDrawing for each generated view. The link point to the object used to create the view (CATPart or CATProduct) |
Conclusion
The design of the table has illustrated five types of links: CCP, KWE, instance, assembly constraint and ViewLink. There are many other types of links, such as MML, Material, Shape, etc. The next article will present the ‘design in context’, which involves context and import links.
SimDesigner Fatigue for CATIA V5: Fatigue Analysis for the Analyst, Part 2
Adarsh Pun, Mark Bacchetti, and Antoine Reymond, MSC.Software Corporation
MSC.Software offers a fully-embedded fatigue analysis solution for CATIA V5 called SimDesigner Fatigue (SFA). SFA is an easy-to-use, integrated solution for design-engineers and analysts who want the advantage of enhanced collaboration in the CATIA V5 environment.
Part 1 of this article describes how a design-engineer can utilize SimDesigner Fatigue during the early stages of product design. SFA essentially provides a “three-step”, initial fatigue solution, where all of the default (“intelligent”) fatigue analysis parameters are set for a “first-run”, robust solution. For deeper fatigue investigations or advanced users, all of the fatigue analysis parameters can be manipulated for further examination of the part.
Part 2 will examine the final stages of product development where the design-engineer and analyst need to work together to optimize the part or product assembly and perform some additional fatigue investigation of the design. SimDesigner Fatigue’s embedded CATIA V5 user interface creates an ideal working environment for this stage in the process when design-engineers, analysts, and managers demand flexibility, collaboration, and productivity.
Continuing from Part 1, the design-engineer performed a simple durability analysis on an ATV lower control arm using most of the “intelligent” solution defaults available in SimDesigner Fatigue. See figure 1. While this analysis identifies the critical hot spots in the structure, an analyst may now want to utilize this analysis to perform a comprehensive durability examination using the advanced loading and solver features of SFA. The integrated solution (CATIA V5 and SFA) allows the analyst to perform a durability assessment without transferring any data to an external software package.
Figure 1: SimDesigner Fatigue process flow.
SimDesigner Fatigue provides the analyst with powerful features that are needed to perform durability assessments. The analyst can perform a comprehensive fatigue analysis by using the following six steps:
1. Create Critical Groups.
2. Create a Fatigue Material.
3. Insert a Fatigue Case.
4. Create or import load time histories for multi channel loading.
5. Select Solution Parameters.
6. Compute and review computed life. |
After completing this process, the design-engineer or analyst can use SimDesigner’s generative capabilities to redesign areas that have been identified with potential failure modes. Let us take a closer look at these six steps to perform advanced fatigue analysis with respect to the lower control arm model above.
1. Create Critical Fatigue Groups
The user has an option to customize groups for a fatigue analysis. See figure 2. By default, all elements and nodes are contained in the Default Group.1. However, if the model is large, it can be sub-divided into groups or grouped by Materials, as indicated in the form below. In this case, the analyst chooses to perform a fatigue analysis on 25% of the highest stressed nodes from the linear static solution.
Figure 2: Creating a group for critical areas.
2. Create a Fatigue Material
Right click on the “Isotropic Material.1” and select Fatigue Material. See figure 3. A dialog box is displayed to allow the User to create fatigue materials data using either the basic or the advanced material properties. For advanced properties, the analyst is required to enter the fatigue material parameters (slopes, exponents, etc). The data can either be entered on the form or imported from an existing *.mat file.
Figure 3: Creating a Fatigue Material.
3. Insert Fatigue Case
Insert a "SD Fatigue Case" and select a SimDesigner Linear Static Case Solution. The fatigue analysis will use the stress results associated with the Linear Static Case for performing a Fatigue analysis at the default element centroid location. The user has the option of changing the results location to nodal or element nodal. In figure 4 below, the nodal results location has been chosen.
Figure 4: Referencing a linear static analysis to a Fatigue Case.
4. Create Multi-Channel Loading Events
SimDesigner Fatigue has two default time histories available: fully reversed constant amplitude and unit (0-1-0). The user can override the default time histories by defining a load time history for each fatigue channel. The default or user created load time histories are then used to create fatigue events, which are the time histories with user defined scale and offset factors applied to them. See figure 5.
Figure 5: Creating events based on realistic time histories.
Once the events have been created, the user can manage the events by specifying if they are to be concatenated or superimposed at all analysis locations. In figure 6 below, superposition of three events is shown. The events can be further modified with a normalizing load, scale factor, and an offset, that provides the analyst more flexibility in achieving the correct loading on the model.
Figure 6: Managing multiple events in SimDesigner Fatigue.
5. Manage Solution Parameters
Selecting the Advanced check box allows the user access to several solver solution parameters, such as mean stress, biaxiality corrections, and factor of safety calculations. The default values will be acceptable for most fatigue analyses. The user is also provided with an opportunity to change the analysis results location (element centroid, element nodes, or nodes) that was selected when inserting the fatigue case. The layer (top, middle, and bottom) position for shell results may also be selected from this form. If the Advanced check box is not selected, no additional user input is required on this form (see figure 7).
The analysis properties also have options for group assignments. Here, the user can manage the groups created from step one. See figure 7. Each group can be modified with different surface conditions, materials, and stresses.
Figure 7: Fatigue solution parameters and group assignments
6. Compute and Review Computed Life
Once the analysis has completed, the user can assess the fatigue by selecting the SimDesigner Fatigue Case Solution. See figure 8.
Figure 8: SimDesigner Fatigue Computation Process.
SimDesigner Fatigue offers a complete set of post-processing plots for the analyst. Plots include Log Life, Damage, Confidence, and Angle Spread. Figure 9 shows the results “Image Generation” selection menu.
Figure 9: Image Generation.
The analyst can now assess the lower control arm’s durability and make recommendations for an improved design. See figure 10. The analyst or design-engineer can modify the part in the CATIA V5 Part Design workbench and immediately compute for a new solution.
Figure 10: Design Iteration with SimDesigner Fatigue.
SimDesigner Fatigue’s integrated solution offers the flexibility needed by the design-engineers and analysts during the design iteration process. By using SimDesigner for CATIA V5, the analyst has the option to quickly iterate the geometry. Likewise, the design-engineer can capture the analyst’s durability process in the final design iterations. This flexibility allows design-engineers and analysts to have improved collaboration that enhances development productivity.
For more information on SimDesigner Fatigue and SimDesigner for CATIA V5, please visit the following websites:
SimDesigner Homepage
SimDesigner Fatigue
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