NX CAM 11: Teach Feature Mapping and Operation Sets

Transcription

1 Siemens PLM Software NX CAM 11: Teach Feature Mapping and Operation Sets Teach NX to apply specific sets of operations to specific feature types. Answers for industry.

2 About NX CAM NX TM CAM software has helped many of the world s leading manufacturers and job shops produce better parts faster. You can also achieve similar benefits by making use of the unique advantages NX CAM offers. This is one of many hands-on demonstrations designed to introduce you to the powerful capabilities in NX CAM 11. In order to run this demonstration, you will need access to NX CAM 11. Visit the NX Manufacturing Forum to learn more, ask questions, and share comments about NX CAM. 2

3 Hands-on Demonstration: Operation Teaching You can now Teach Feature Mapping and Teach Operation Sets. The ability to create mapping and machining rules is particularly useful when specific machining workflows are required and must be applied consistently to commonly used feature types. In this self-demo, you will first teach NX to map the standard feature types to those commonly used in your specific work environment. You will then teach operation sets and apply the machining rules to machine a part. 3

4 Prerequisites: 1. You will need access to NX CAM 11 in order to run this demonstration. 2. If you haven t done so already, download and unzip teach_feature_mapping_and_operation_sets.7z. Note: You must have write permissions for your machining knowledge library and a Machining Knowledge Editor Author license to teach the feature mappings and operation sets. We recommend that you make a backup copy of your machining knowledge library before you try this workflow. To do this, go to Menu Help Log File and find UGII_CAM_MACHINING_KNOWLEDGE_DIR. This will tell you where your machining knowledge library is located. Example: D:\workdir\groups\nx11\wntx64\kits\mach\resource\machining_knowledge\ Find the machining_knowledge folder and copy it. Turn Read-only off for the machining_knowledge folder. Keep the machining_knowledge Copy folder as your readonly backup. When finished with this tutorial, delete the machining_knowledge folder and rename the machining_knowledge Copy folder back to machining_knowledge. Demo: 1. Open teach.prt in NX. 2. Save a copy of this part and rename it my_teach.prt. You will use this copied part to create the rules. You will then apply these rules to another part that you will machine. 4

5 Recognize the features you will use to create mapping rules Recognizing the features you will use to create the mapping rules is optional. By doing this however, NX sets the input type in the Teach Feature Mapping dialog box to match the feature that you selected to teach and you can look at the feature's parameter values 1. In the Machining Features Navigator, right-click and select Find Features. 2. Specify the following: 3. Click Select Face. 4. Select the four faces. 5. Click Find Features. 6. Click OK. 5

6 Create a mapping rule that maps all holes with any color except Yellow (color #6) to the feature type STANDARD_HOLE 1. In the Machining Feature Navigator, right-click STEP1HOLE_1 and select Teach Feature Mapping. In the Feature Type Mappings section of the dialog box, the selected Input and Output types default to STEP1HOLE because you began by selecting the STEP1HOLE_1 feature. 2. Click Add New Type. 3. Type STANDARD_HOLE as the new Output Type. 6

7 4. Select Mapping at the top of the Select Rule list. 5. Click Add New Rule. 6. Type MAP_2_STANDARD_HOLE in the Select Rule list. 7

8 7. Specify the following as the mapping conditions: a. In the Objects list, select STEP1HOLE. b. In the Parameters list, select COLOR. c. In the Operators section, click. d. Type Click Validate. This mapping rule describes when a feature, which originally was labeled as a STEP1HOLE ( in ), should be transferred into a feature of type STANDARD_HOLE ( out ). This rule will map all holes with any color except #6 (yellow) to the STANDARD_HOLE feature type. 9. Click Teach Mapping Rule. 10. Click OK. The MAP_2_STANDARD_HOLE rule with the condition in.color<>6 has been written to the machining knowledge library. 8

9 Create a mapping rule that will map all holes with only Yellow (color #6) to the feature type TOLERANCED_HOLE 1. In the Machining Feature Navigator, right-click STEP1HOLE_2 and select Teach Feature Mapping. 2. Click Add New Type. 3. Type TOLERANCED_HOLE as the new Output Type. 4. Select Mapping at the top of the Select Rule list. 5. Click Add New Rule. 9

10 6. Type MAP_2_TOLERANCED_HOLE_COLOR in the Select Rule list. 7. Specify the following as the mapping conditions: a. In the Objects list, select STEP1HOLE. b. In the Parameters list, select COLOR. c. In the Operators section, click. d. Type 6. 10

11 8. Click Validate. This mapping rule describes when a feature, which originally was labeled as a STEP1HOLE ( in ), should be transferred into a feature of type TOLERANCED_HOLE ( out ). This rule will map all holes with the color #6 (yellow) to the TOLERANCED_HOLE feature type. 9. Click Teach Mapping Rule. The MAP_2_TOLERANCED_HOLE_COLOR rule with the condition in.color=6 will be written to the machining knowledge library when you click OK. As long as you do not click Apply or OK, you can cancel your updates if you make a mistake. If you need to delete a mapping rule after saving it to the machining knowledge library, use the Machining Knowledge Editor application. You will define several more rules and then click OK once to write them to the machining knowledge library. Create a second mapping rule for the TOLERANCED_HOLE feature type that will map all holes with ISO class <=7 1. With TOLERANCED_HOLE still selected in the Select Output Type list, select Mapping at the top of the Select Rule list. 2. Click Add New Rule in the Select Rule list. 3. Type MAP_2_TOLERANCED_HOLE_PMI in the Select Rule list. 4. Specify the following: a. In the Operators section, click the function button. The Fx button lists all functions that can be used within operation set teaching and Teach Feature Mapping for those cases where more complex mathematics are needed. b. In the Functions list, select IT_class_ISO. c. In the Objects list, select STEP1HOLE. d. In the Parameters list, select DIAMETER_1 e. Type a comma. f. In the Parameters list, expand DIAMETER_1 and select UPPER. g. Type a comma. h. In the Parameters list, select LOWER. i. Click. j. Click. k. Type 7. 11

12 5. Click Validate. This mapping rule describes when a feature, which originally was labeled as a STEP1HOLE ( in ), should be transferred into a feature of type TOLERANCED_HOLE ( out ). This rule will map all holes with tolerance class 7 or lower (like H7 ) to the TOLERANCED_HOLE feature type. 6. Click Teach Mapping Rule. Create a third mapping rule for the TOLERANCED_HOLE feature type that will map all holes with the face attribute MW_HOLE_FIT 1. With TOLERANCED_HOLE still selected in the Select Output Type list, select Mapping at the top of the Select Rule list. 2. Click Add New Rule in the Select Rule list. 3. Type MAP_2_TOLERANCED_HOLE_FACE in the Select Rule list. 4. Specify the following: a. In the Operators section, click. b. In the Functions list, select is_defined. c. In the Objects list, select STEP1HOLE. d. In the Parameters list, select MW_HOLE_GUIDE_PIN_FIT. e. Click. 5. Click Validate. This rule will map all holes with the MW_HOLE_GUIDE_PIN_FIT attribute to the TOLERANCED_HOLE feature type. 6. Click Teach Mapping Rule. 12

13 Prioritize mapping rules NX uses the priority together with the conditions to determine which feature to map. A larger priority number indicates a higher priority. If you do not assign a priority, NX applies the first rule selected at random which has all of its conditions satisfied. 1. Select MAP_2_TOLERANCED_HOLE_COLOR mapping rule in the Select Rule list. 2. Select the More tab. 3. Type 100 in the Priority box and press Enter. 4. Click Teach Mapping Rule. 5. Select MAP_2_TOLERANCED_HOLE_PMI in the Select Rule list. 6. Type 100 in the Priority box and press Enter. 7. Click Teach Mapping Rule. 8. Select MAP_2_TOLERANCED_HOLE_FACE in the Select Rule list. 9. Type 100 in the Priority box and press Enter. 10. Click Teach Mapping Rule. 11. Click OK in the Teach Feature Mapping dialog box. The MAP_2_TOLERANCED_HOLE_COLOR, MAP_2_TOLERANCED_HOLE_PMI, and MAP_2_TOLERANCED_HOLE_FACE rules have been written to the machining knowledge library. 13

14 Create the operation sets You will use the 4 holes to the right of the slot to create the following operation sets. STANDARD_HOLE_DRILL_TO_SIZE to drill a hole to size when the matching drill is available. STANDARD_HOLE_MILL_TO_SIZE to drill a hole and then mill it to size when a matching drill is not available. TOLERANCED_HOLE_BORE to drill a hole and then bore it to tolerance. TOLERANCED_HOLE_REAM to drill a hole and then bore and ream to tolerance. You will begin by recognizing the four holes used to create the operation sets. 1. In the background of the Machining Feature Navigator, MB3 Find Features. 2. Specify the following: a. Type: Parametric Recognition b. Search Method: All Geometry c. Map Features d. Mapping STANDARD_HOLE e. Mapping TOLERANCED_HOLE f. Recognition g. Method: None h. Assign Color Attribute 3. Click Find Features. 14

15 4. Click OK. Create the feature groups that will contain the operation sets 1. In the Machining Feature Navigator, right-click STANDARD_HOLE_3 and select Group Features. 2. Click Create Feature Groups. 3. Click OK. 4. In the Machining Feature Navigator, right-click STANDARD_HOLE_5 and select Group Features. 5. Click Create Feature Groups. 6. Click OK. 7. Right-click TOLERANCED_HOLE_4 and select Group Features. 8. Click Create Feature Groups. 9. Click OK. 10. Right-click TOLERANCED_HOLE_6 and select Group Features. 11. Click Create Feature Groups. 12. Click OK. 15

16 13. Display the Geometry View of the Operation Navigator and rename the feature groups. 14. Save the part. Create the operations for each feature group as you normally would 1. For this exercise, copy the operations from operations.prt. 2. Generate the tool paths. 3. Save my_teach.prt. 16

17 Teach the STANDARD_HOLE_DRILL_TO_SIZE operation set Next, you will teach feature conditions to the STANDARD_HOLE_DRILL_TO_SIZE operation set. Feature conditions determine the features to which the operation sets will be applied. You will begin by assigning a higher priority to the STANDARD_HOLE_DRILL_TO_SIZE operation set so that NX will drill before milling. 1. In the Geometry View of the Operation Navigator, select the two STANDARD_HOLE feature groups and right-click Object Teach Operation Sets. 2. In the Operation Sets list, select the STANDARD_HOLE_DRILL_TO_SIZE feature group. 3. Select the More tab. 4. Type 100 in the Priority box and press Enter. 5. Select the Conditions tab. Now you will specify a condition that applies this operation set to any STANDARD_HOLE feature with a depth that is less than 6 times the diameter. 6. Specify the following as the application conditions: a. In the Objects list, select STANDARD_HOLE. b. In the Parameters list, select DEPTH. c. In the Operators section, click. d. In the Parameters list, select DIAMETER_1. e. In the Operators section, click. f. Type 6. 17

18 7. Click Validate. This condition specifies that the STANDARD_HOLE_DRILL_TO_SIZE operation set will be applied to any STANDARD_HOLE feature with a depth that is less than 6 times the diameter 8. Click Teach Machining Rules. 18

19 Specify tool selection conditions for DRILLING operations You will now specify the tool selection conditions for drilling operations that will drill standard holes to size. 1. In the Operation Sets list, select the DRILLING operation. 2. Specify the following as the tool selection conditions: a. In the Objects list, select tool. b. In the Parameters list, select (D)DIAMETER. c. In the Operators section, click. d. In the Objects list, select STANDARD_HOLE. e. In the Parameters list, select DIAMETER_1. f. Click Validate. This condition specifies that the drilling tool diameter must be equal to the feature diameter. NX will select the largest tool in the class that satisfies these conditions. g. In the Objects list, select tool. h. In the Parameters list, select (FL)Flute Length. i. Click. j. In the Objects list, select STANDARD_HOLE. k. In the Parameters list, select DEPTH. l. Click Validate. This condition specifies that the flute length must be greater than the feature depth. 3. Click Teach Machining Rules. 19

20 Specify tool selection conditions for COUNTERSINKING operations You will now specify the tool selection conditions for countersinking the standard holes that have been drilled to size. This describes which specific countersink tool should be selected for this operation based on the feature dimensions. 1. In the Operation Sets list, select the COUNTERSINKING operation. 2. Specify the following as the tool selection conditions: a. Objects list: tool b. Parameters list: (TD) TIP DIAMETER c. Click. d. Objects list: STANDARD_HOLE e. Parameters list: DIAMETER_1 f. Click Validate. This condition specifies that the countersinking tool tip diameter must be less than the feature diameter. In other words, the tool tip must fit into the hole. NX will select the largest tool in the class that satisfies this condition. g. Objects list: tool h. Parameters list: (D) DIAMETER i. Click. j. Type 2 k. Click. l. Objects list: STANDARD_HOLE m. Parameters list: DIAMETER_1 n. Click Validate. This condition specifies that the large countersinking tool diameter must be less than twice the feature diameter. In other words, the large tool diameter should be larger than the feature diameter, but also not too large. 3. Click Teach Machining Rules. 20

21 Teach the STANDARD_HOLE_MILL_TO_SIZE operation set You will now teach feature conditions to the STANDARD_HOLE_MILL_TO_SIZE operation set. 1. In the Operation Sets list, select the STANDARD_HOLE_MILL_TO_SIZE feature group. 2. Specify the following as the application conditions: a. Objects list: STANDARD_HOLE b. Parameters list: DEPTH c. Click. d. Parameters list: DIAMETER_1 e. Click. f. Type 6. g. Click Validate. This condition specifies that the STANDARD_HOLE_MILL_TO_SIZE operation set will be applied to any STANDARD_HOLE feature with a depth that is less than 6 times the diameter. 3. Click Teach Machining Rules. 21

22 Specify tool selection conditions for PRE-DRILLING operations You will now specify the tool selection conditions for operations that will pre-drill standard holes prior to milling. 1. In the Operation Sets list, select the PRE-DRILLING_1 operation. 2. Specify the following as the tool selection conditions: a. Objects list: tool. b. Parameters list: (D)DIAMETER c. Click. d. Objects list: STANDARD_HOLE e. Parameters list: DIAMETER_1 f. Click Validate. This condition specifies that the drilling tool must be smaller than the feature diameter. NX will select the largest tool in the class that satisfies this condition. 3. Click Teach Machining Rules. 22

23 Specify tool selection conditions for the HOLE_MILLING operation You will now specify the tool selection conditions for operations that will mill the pre-drilled standard holes to size. 1. In the Operation Sets list, select the HOLE_MILLING _1 operation. 2. Specify the following as the tool selection conditions: a. Objects list: tool b. Parameters list: (D)DIAMETER c. Click. d. Objects list: STANDARD_HOLE e. Parameters list: DIAMETER_1 f. Click. g. Type 0.85 h. Click Validate. The above condition specifies that the milling tool must be smaller than 85% of the feature diameter. NX will select the largest tool in the class that satisfies these conditions. 3. Click Teach Machining Rules. 23

24 Specify tool selection conditions for CHAMFER_MILLING operations You will now specify the tool selection conditions for operations that will chamfer mill standard holes. 1. In the Operation Sets list, select the HOLE_CHAMFER_MILLING_1 operation. 2. Specify the following as the tool selection conditions: a. Objects list: tool b. Parameters list: (D)DIAMETER c. Click. d. Objects list: STANDARD_HOLE e. Parameters list: DIAMETER_1 f. Click. g. Type 0.85 h. Click Validate. The above condition specifies that the chamfer tool must be smaller than 85% of the feature diameter. NX will select the largest tool in the class that satisfies these conditions. 3. Click Teach Machining Rules. 4. Click OK to save the rules to the Machining Knowledge Library and close the dialog box. 24

25 Teach the TOLERANCED_HOLE_REAM operation set You will now teach feature conditions to the TOLERANCED_HOLE_REAM operation set. 1. In the Geometry View of the Operation Navigator, select the two TOLERANCED_HOLE feature groups and right-click Object Teach Operation Sets. 2. In the Operation Sets list, select the TOLERANCED_HOLE_REAM feature group. 3. Specify the following as the application conditions: a. Objects list: TOLERANCED_HOLE b. Parameters list: DEPTH c. Click. d. Parameters list: DIAMETER_1 e. Click. f. Type 6. g. Click Validate. This condition specifies that the TOLERANCED_HOLE_REAM operation set will be applied to any TOLERANCED_HOLE feature with a depth that is less than 6 times the diameter. h. Click. i. Functions list: IT_class_ISO j. Objects list: TOLERANCED_HOLE k. Parameters list: DIAMETER_1 l. Type a comma. m. Parameters list: expand DIAMETER_1 and select UPPER. n. Type a comma. o. Parameters list: LOWER 25

26 p. Click. q. Click. r. Type 5. s. Click Validate. This condition specifies that the TOLERANCED_HOLE_REAM operation set will be applied to any TOLERANCED_HOLE feature with a diameter tolerance grade up to Click Teach Machining Rules. 26

27 Specify tool selection conditions for DRILLING operations You will now specify the tool selection conditions for operations that will drill toleranced holes to less than the feature diameter. 1. In the Operation Sets list, select the DRILLING_T_1 operation. 2. Specify the following as the tool selection conditions: a. Objects list: tool b. Parameters list: (D)DIAMETER c. Click. d. Objects list: TOLERANCED_HOLE e. Parameters list: DIAMETER_1 f. Press the space bar. Note: You must always add a space before and after the operators - and +. g. Click. h. Press the space bar. i. Type 2.0 j. Click Validate. This condition specifies that the drilling tool must be 2.0mm smaller than the feature diameter. NX will select the largest tool in the class that satisfies this condition. k. Objects list: tool l. Parameters list: (FL)Flute Length m. Click. n. Objects list: TOLERANCED_HOLE o. Parameters list: DEPTH p. Click Validate. This condition specifies that the flute length must be greater than the feature depth. 3. Click Teach Machining Rules. 27

28 Specify tool selection conditions for BORING operations You will now specify the tool selection conditions for operations that will bore toleranced holes to less than the feature diameter. A tool tolerance range is defined by an upper and lower limit. 1. In the Operation Sets list, select the BORE_T1 operation. 2. Specify the following as the tool selection conditions: a. Objects list: tool. b. Parameters list: (D)DIAMETER c. Click. d. Objects list: TOLERANCED_HOLE e. Parameters list: DIAMETER_1 f. Press the space bar. g. Click. h. Press the space bar. i. Type 0.15 j. Click Validate. k. Objects list: tool l. Parameters list: (D)DIAMETER m. Click. n. Objects list: TOLERANCED_HOLE o. Parameters list: DIAMETER_1 p. Press the space bar. q. Click. r. Press the space bar. s. Type 0.2 t. Click Validate. 3. Click Teach Machining Rules. 28

29 Specify tool selection conditions for COUNTERSINKING operations You will now specify the tool selection conditions for countersinking toleranced holes that have been bored to size. 1. In the Operation Sets list, select the COUNTERSINKING_T_1 operation. 2. Specify the following as the tool selection conditions: a. Objects list: tool b. Parameters list: (TD) TIP DIAMETER c. Click. d. Objects list: TOLERANCED_HOLE e. Parameters list: DIAMETER_1 f. Click Validate. This condition specifies that the countersinking tool tip diameter must be less than the feature diameter. In other words, the tool tip must fit into the hole. NX will select the largest tool in the class that satisfies this condition. g. Objects list: tool h. Parameters list; (D) DIAMETER i. Click. j. Type 2. k. Click. l. Objects list: TOLERANCED _HOLE m. Parameters list: DIAMETER_1 n. Click Validate. This condition specifies that the large countersinking tool diameter must be less than twice the feature diameter. In other words, the large tool diameter should be larger than the feature diameter, but also not too large. 3. Click Teach Machining Rules. 29

30 Specify tool selection conditions for REAMING operations You will now specify the tool selection conditions for operations that will ream toleranced holes to the feature diameter. 1. In the Operation Sets list, select the REAM_T1 operation. 2. Specify the following as the tool selection conditions: a. Objects list: tool b. Parameters list: (D)DIAMETER c. Click. d. Objects list: TOLERANCED_HOLE e. Parameters list: DIAMETER_1 f. Click Validate. This condition specifies that the reaming tool diameter must equal the feature diameter. g. Objects list: tool h. Parameters list: (FL)Flute Length i. Click. j. Objects list: TOLERANCED_HOLE k. Parameters list: DEPTH l. Click Validate. This condition specifies that the flute length must be greater than the feature depth. 3. Click Teach Machining Rules. 30

31 Teach the TOLERANCED_HOLE_BORE operation set You will now teach feature conditions to the TOLERANCED_HOLE_BORE operation set. 1. In the Operation Sets list, select the TOLERANCED_HOLE_BORE feature group. 2. Specify the following as the application conditions: a. Objects list: TOLERANCED_HOLE b. Parameters list: DEPTH c. Click. d. Parameters list: DIAMETER_1 e. Click. f. Type 6. g. Click Validate. This condition specifies that the TOLERANCED_HOLE_BORE operation set will be applied to any TOLERANCED_HOLE feature with a depth that is less than 6 times the diameter. h. Click. i. Functions list: IT_class_ISO j. Objects list: TOLERANCED_HOLE k. Parameters list: DIAMETER_1 l. Type a comma. m. Parameters list: expand DIAMETER_1 and select UPPER. n. Type a comma. o. Select LOWER. p. Click. q. Click. r. Type 5. s. Click Validate. This condition specifies that the TOLERANCED_HOLE_BORE operation set will be applied to any TOLERANCED_HOLE feature with a diameter tolerance grade up to 5. 31

32 3. Click Teach Machining Rules. Specify tool selection conditions for DRILLING operations You will now specify the tool selection conditions for operations that will drill toleranced holes to less than the feature diameter. 1. In the Operation Sets list, select the DRILLING_T_2 operation. NX automatically copies these conditions from the DRILLING_T_1 operation because they are exactly the same. There is no need to teach the mapping rule for this operation. Specify tool selection conditions for BORING operations You will now specify the tool selection conditions for operations that will bore toleranced holes to the feature diameter. 1. In the Operation Sets list, select the BORE_T2 operation. 2. Specify the following as the tool selection conditions: a. Objects list: tool b. Parameters list: (D)DIAMETER c. Click. d. Objects list: TOLERANCED_HOLE e. Parameters list: DIAMETER_1 f. Click Validate. This condition specifies that the boring tool diameter must equal the feature diameter. 3. Click Teach Machining Rules. 32

33 Specify tool selection conditions for COUNTERSINKING operations You will now specify the tool selection conditions for countersinking toleranced holes that have been bored to size. 1. In the Operation Sets list, select the COUNTERSINKING_T_2 operation. Again, NX automatically copies these conditions from the COUNTERSINKING_T_1 operation because the operations are exactly the same. There is no need to teach the mapping rule for this operation. 2. Click OK in the Teach Operation Sets dialog box. This completes the process of defining geometry conditions for operation sets and tool selection conditions for operations. 3. Save and close the part. 33

34 Use STANDARD_HOLE and TOLERANCED_HOLE feature types to create the feature process You will now use the feature conditions and the tool selection conditions you defined in the operation sets to create the workflow in a test part. 1. Open test.prt 2. Make sure that the Display Information During Feature Mapping and Group Creation customer default is turned on. This will help you to troubleshoot any issues you find during testing. a. File Utilities Customer Defaults b. Select Geometry in the left column under Manufacturing. c. Select the Features tab. d. Display Information During Feature Mapping and Group Creation e. Click OK. 3. In the Machining Feature Navigator, MB3 Find Features. 4. Specify the following: a. Type: Parametric Recognition b. Search Method: All Geometry c. Map Features d. Mapping STANDARD_HOLE e. Mapping TOLERANCED_HOLE f. Recognition g. Method: None h. Assign Color Attribute 5. Click Find Features. 6. Click OK. 34

35 7. Right-click on one of the selected features and choose Create Feature Process. 8. Specify the following: a. Type: Rule Based b. Machining Knowledge Operation Sets c. Geometry: Automatic d. Groups: Use Existing 9. Click OK. 10. Display the Geometry View of the Operation Navigator. 11. Generate the tool paths. 12. Close the part without saving. 35

36 Siemens Industry Software Headquarters Granite Park One 5800 Granite Parkway Suite 600 Plano, TX USA Americas Granite Park One 5800 Granite Parkway Suite 600 Plano, TX USA Europe Stephenson House Sir William Siemens Square Frimley, Camberley Surrey, GU16 8QD +44 (0) Asia-Pacific Suites , 43/F AIA Kowloon Tower, Landmark East 100 How Ming Street Kwun Tong, Kowloon Hong Kong About Siemens PLM Software Siemens PLM Software, a business unit of the Siemens Industry Automation Division, is a leading global provider of product lifecycle management (PLM) software and services with seven million licensed seats and more than 71,000 customers worldwide. Headquartered in Plano, Texas, Siemens PLM Software works collaboratively with companies to deliver open solutions that help them turn more ideas into successful products. For more information on Siemens PLM Software products and services, visit Siemens Product Lifecycle Management Software Inc. Siemens and the Siemens logo are registered trademarks of Siemens AG. D-Cubed, Femap, Geolus, GO PLM, I-deas, Insight, JT, NX, Parasolid, Solid Edge, Teamcenter, Tecnomatix and Velocity Series are trademarks or registered trademarks of Siemens Product Lifecycle Management Software Inc. or its subsidiaries in the United States and in other countries. All other logos, trademarks, registered trademarks or service marks used herein are the property of their respective holders. 36