Presentation By: Daniel Heaton CATIA V5 Knowledgeware CATIA V5 Workbook * Southern Utah University * Schroff Development Corporation* Corporate Visual Systems Project By: Daniel Heaton Documented by: Richard Cozzens

Lesson Objectives 1.) Introduce CATIA V5 Knowledgeware Work Benches and tools. 2.) Show how CATIA V5 Knowledgeware was used to solve a real life design problem. 3.) Present the process using several different learning methods: 3.1.) Live step by step demonstration. 3.2.) A clear and detailed AVI file of the step by step process for later review. 3.3.) Power Point Presentation highlighting the major steps. 3.4.) A detailed step by step lesson plan with review questions and practice exercises. 3.5.) Supply reference CATPart, CATScript and CATDrawing files. 3.6.) Supply training test for instructors and/or self test. 4.) Conclude by answering questions and/or taking suggestions! Download site: Training AVI, PP Presentation, V5 models:

Knowledgeware Work Benchs & Tools Questions and/or Comments to: Southern Utah University, Cedar City, Utah Knowledgeware is not an individual work bench but several work benches including tools in the Part Design Work Bench

Knowledgeware Putting Part Intelligence To Use Use CATIA V5 Knowledgeware capabilities to: 1) Select the correct Extrusion. 2) Apply specific (custom) joggle dimensions. 3) Check design against company/industry standards. 4) Automatically create a custom Production Drawing. Production requires accurate custom Joggled Extrusion Drawings. No extra time allowed to create the custom Production Drawings. CATIA V5 Workbook * Southern Utah University * Schroff Development Corporation* Corporate Visual Systems The ProblemThe Solution

Step 1 Determine the Requirements What is known? What is not known? What are your variables? What is the Process? Can the process be automated? How can Knowledgeware help? What is the end goal? Extrusion Tables, Joggle Drawings. How to apply Knowledgeware. Extrusion dimensions and joggle dimensions. Create Joggled Extrusion, constrain it, create a Production Drawing, modify constraints as required. Using Design Tables and creating a macro. Automating the macro using VBScript Basic Production Drawing created quickly and accurately. Download site: Training AVI, PP Presentation, V5 models:

Step 2 Creating The Extrusion Profile Sketch Create the Sketch on the ZX Plane. Create the general shape of the L shaped extrusion: a.) Height = 2 in b.) Stand leg thickness =.20 in c.) Length = 2 in d.) Base leg thickness =.25 in Questions and/or Comments to: Southern Utah University, Cedar City, Utah

Step 3 Constraining The Extrusion Profile Sketch CATIA V5 Workbook * Southern Utah University * Schroff Development Corporation* Corporate Visual Systems Constrain the Extrusion Profile Sketch as shown. Be sure to use the correct constraint types.

Step 4 Modifying The Constraint Names 1.) Double click on the constraint. 2.) Select the More Button. 3.) Edit the existing name as required. 4.) Select OK. 5.) The new name will show up in the Specification Tree Download site: Training AVI, PP Presentation, V5 models:

Step 5 Creating The Joggle Profile Sketch Create the Sketch in the ZX Plane. Create general sketch as shown using these dimensions: a.) Transition=5 in b.) Depth =.75 in c.) Dist. To Endp=4 in d.) Length = 5 in Schroff Development Corporation

Step 6 Constraining The Joggle Profile Sketch Constrain the Joggle Profile Sketch as shown. Be sure to use the correct type of constraint. CATIA V5 Workbook * Southern Utah University * Schroff Development Corporation* Corporate Visual Systems

Step 7 Modifying The Constraint Names Modify the constraint names as shown: a.) Transition. b.) Depth. c.) Dist. To Endp. d.) Length.50 Download site: Training AVI, PP Presentation, V5 models:

Step 8 Creating A Solid From The Two Sketches Using The Rib Tool 2.) From the Profile Box select the Extrusion Profile Sketch. 3.) From the Center Curve Box Select the Joggled Profile Sketch. 4.) Select OK. 5.) Notice a Rib.1 appear on the Specification Tree under the PartBody Branch. 1.) Select the Rib Tool Questions and/or Comments to: Southern Utah University, Cedar City, Utah

Step 9 Creating An Extrusion Table CATIA V5 Workbook * Southern Utah University * Schroff Development Corporation* Corporate Visual Systems 1.) Design Tables can be created in CATIA V5 or externally to CATIA V5 using one of the following: a.) Microsoft Excel. b.) Lotus Spread Sheet. c.) A Text File. 2.) Create a spreadsheet using the data below (Extrusion numbers and Dimensions are from the Tierany Metals Catalog):

Step 10 Linking The Extrusion Table 1.) Select the Design Table Tool. 2.) Name the Design Table. 3.) Select the Create a design table from a pre-existing file. 4.) Select Ok. 5.) Locate and select the pre-existing file using the browser. 6.) Select the Open Button. 7.) Select YES to automatically associate columns & parameters. Even though the constraints and columns are named the same a manual association may be required. Download site: Training AVI, PP Presentation, V5 models:

Step 10 (Continued) Manually Associating The Parameters & Columns 8.) Select the Association tab in the Extrusion Table Active Window. 9.) From the Column Box select Extrusion Number 10.) Select the Create Parameters Button (Extrusion Number does not have a constraint equivalent so you must create one, it will be a string type). 11.) Select the Extrusion Number. 12.) Select the OK Button. 13.) In the Extrusion Table Active Window select A from the Columns Box. Corporate Visual Systems

Step 10 (Continued) Manually Associating The Parameters & Columns CATIA V5 Workbook * Southern Utah University * Schroff Development Corporation* Corporate Visual Systems 14.) From the Parameters Box select the …\A\Offset line (Not the …\A\Activity parameter). 15.) Select the Associate Button (the new association will show up in the Association Box. 16.) Associate all the variables in the Columns Box (as shown here). 17.) Select the OK Button.

Step 11 Applying The Design Table To The Joggled Extrusion 1.) Double click on the Extrusion Table Branch in the Specification Tree. This activates the Knowledge Advisor Work Bench. 2.) Double clicking on the Extrusion Table Branch again will open up the Extrusion Table (as shown). 3.) Select row 3. 4.) Select Ok. 5.) Notice the Joggled Extrusion Part will update to the new dimensions. The changes will show up in the Specification Tree. Download site: Training AVI, PP Presentation, V5 models:

Step 11 (Continued) Applying The Design Table To The Joggled Extrusion This is the result of selecting row 3 from the Design Table (Extrusion Table). The Extrusion is automatically updated to your selection. Questions and/or Comments to: Southern Utah University, Cedar City, Utah

Step 12 Editing The Extrusion Table 3.) Edit the table in the original spread sheet. 4.) Save the changes. 5.) Exit the spread sheet program. 6.) Select OK to update the extrusion. 1.) Enter the Extrusion Table as explained in Step 11. CATIA V5 Workbook * Southern Utah University * Schroff Development Corporation* Corporate Visual Systems 2.) Select the Edit Table Button.

Step 13 Displaying The Extrusion Type In the Specification Tree 1.) Select Tools (top Tool Bar). 2.) Select Options (Tree). 3.) Select Parameters (Under General Branch). 4.) Select Knowledge (Tab). 5.) Go to Parameters Tree View (Section). 6.) Select the With Value. Notice: Material Type and Extrusion Number show up (from the Extrusion Table). Download site: Training AVI, PP Presentation, V5 models:

Step 14 Modifying The Existing Joggled Profile Sketch Currently you can go into the Joggle Profile Sketch and manually revise the constraints as shown. The resulting Joggled Extrusion.CATPart is also shown. Schroff Development Corporation

Step 15 Automating The Modification Using A Marco CATIA V5 Workbook * Southern Utah University * Schroff Development Corporation* Corporate Visual Systems 6.) Exit the Sketcher Work Bench. 7.) Select Stop Recording. 8.) Name the Macro JoggleDimension.CATScript. 1.) Enter the Joggle Profile Sketch. 2.) Select Tools (Top Tool Bar). 2.) Select Macro. 3.) Select Start Recording. 4.) Select the Start Button. 5.) Manually change the constraints as shown.

Step 15 (Continued) Automating The Modification Using A Marco Notice: The Joggled Extrusion changes to the values you set when recording the macro. Test the Macro: 1.) Change the constraint values so they are different. 2.) Select Tools, Macro 3.) Select the Macro. 4.) Select Run. Download site: Training AVI, PP Presentation, V5 models:

Step 16 Customizing The Macro Using VBScript 1.) Select Tools. 2.) Select Macro. 3.) Select the Joggle Dimensions.CATScript Macro. 4.) Select the Edit Button. 5.) This will bring up the VBScript Edit Window as shown on the following slide. Questions and/or Comments to: Southern Utah University, Cedar City, Utah

Step 16 (continued) Customizing The Macro Using VBScript CATIA V5 Workbook * Southern Utah University * Schroff Development Corporation* Corporate Visual Systems First Constraint that was revised (Transition) from 4.0 to 2.5 Note: VBScript shows up in mm. Second Constraint that was revised (Depth) from.75 to 1.0. Third Constraint that was revised (Joggle Location) from 4.0 to 2.5.

Step 16 (continued) Customizing The Macro Using VBScript Add these three lines at line 54 to Prompt the user for input for Joggle location, Transition and Depth. Replace the value of Length1 with Transition*(25.4) variable. Replace the value of Length2 with Depth*(25.4) variable. Replace the value of Length3 with Jogglelocation*(25.4) variable. Download site: Training AVI, PP Presentation, V5 models:

Step 17 Creating Input Windows Using VB Script Add these three lines of code in the location shown. Corporate Visual Systems

Step 17 (continued) Creating Input Windows Using VB Script CATIA V5 Workbook * Southern Utah University * Schroff Development Corporation* Corporate Visual Systems The resulting Input boxes pop up one after another until all three variables are assigned a value. The constraints are updated and the Joggled Extrusion.CATPart is updated accordingly.

Step 18 Creating A Tool Icon For The Macro 1.) Select Tools. 2.) Select Customize. 3.) Select Commands (tab). 4.) Select Macros. 5.) *.CATScript files will show up. 6.) Drag and drop the CATScript on a Tool Bar. 7.) Tool Icon is now ready to be selected and run. Download site: Training AVI, PP Presentation, V5 models:

Step 19 Practical Application… Creating An Up To Date Production Drawing Automatically 1.) Create a simple Production Drawing with 3 orthographic views and 1 isometric view. 2.) Dimension the joggle values, not the extrusion, the extrusion dimensions are in the Tierany Metal Catalog. 3.) Add title block and notes as required. 4.) Any time the Joggled Extrusion CATPart is updated using the table and/or the Joggle CATScript the Production Drawing will automatically update also, thus automating the process. Reference the next slide for an example! Schroff Development Corporation

Step 19 (Continued) Practical Application… Creating An Up To Date Production Drawing Automatically CATIA V5 Workbook * Southern Utah University * Schroff Development Corporation* Corporate Visual Systems

Step 20 Applying Company & Industry Standards/Knowledge Using The Check Tool 1.) Double click on the Relations Branch of the Specification Tree to bring up the Knowledge Advisor Work Bench. 2.) Select the Check Tool. 3.) Name the Check: JoggleRatio. 4.) Create the check: The Joggle can not be more than ¼ (Rise/run) select the constraints; (Transition/Depth>=4. 5.) Type of Check is Information. 6.) Enter Message: The Depth Ratio must be less than 1 to 4! 7.) Select OK to create. 8.) Test the Check, enter 3,1,1. Download site: Training AVI, PP Presentation, V5 models:

Step 20 (Continued) Applying Company & Industry Standards/Knowledge Using The Check Tool 11.) The part will still update to the numbers entered, but you were warned and there is a message in the Specification Tree. 9.) The JoggleRatio Warning Window will appear. 10.) A red light will show up in the Relations Branch of the Specification Tree. Questions and/or Comments to: Southern Utah University, Cedar City, Utah

Knowledgeware Summary > Knowledgeware is a very powerful tool. > The Joggled Extrusion is a basic application of Knowledgeware but has proven to be a big time saver. > Now that you understand the basics you can apply these tools to more complex problems. > Knowledgeware is limited only by your imagination. CATIA V5 Workbook * Southern Utah University * Schroff Development Corporation* Corporate Visual Systems

Acknowledgments Project Development:Daniel Heaton Project Manager:Richard Cozzens Documentation:Richard Cozzens Presentation:Daniel Heaton Project Support:Southern Utah University Metalcraft Technologies, Inc. Presentation Support:CATIA V5 Workbook Schroff Development Corp. Corporate Visual Systems H.E.A.T. COE Questions and/or DownLoad site: Training AVI File Power Point Presentation, CATIA V5 models: htm CATIA V5 Workbook * Southern Utah University * Schroff Development Corporation* Corporate Visual Systems