Siemens PLM Software More efficient hole drilling with feature recognition NX CAM 9: How to apply new feature groups to the new manual drilling operations Answers for industry.
About NX CAM NX TM CAM software has helped many of the world s learning 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 9. In order to run this demonstration, you will need access to NX CAM 9. Visit the NX Manufacturing Forum to learn more, ask questions, and share comments about NX CAM. 2
Hands-on Demonstration: More efficient hole drilling with feature recognition This enhancement provides new operation subtypes for hole making operations and the ability to group features based on the feature type. Do you have a question? Post your questions or comments at the bottom of this Tech Tip article in the NX Manufacturing Forum. 3
Prerequisites: 1. You will need access to NX CAM 9 in order to run this demonstration. 2. If you haven t done so already, download and unzip Manual Drilling Operation parts.7z. You will find the.7z file attached directly to this Tech Tip article in the NX Manufacturing Forum. Demo: 1. Open drilling.prt in NX. Geometry Definition You will begin by defining geometry for manual drilling operations using feature recognition and subsequent feature groups. 2. Display the Machining Feature Navigator. 3. In the background of the Machining Feature Navigator, MB3 Find Features. 4. Select Parametric Recognition from the Type list. 5. Click Recognition to clear the box. 6. Scroll down and click STEPS to select it. This will cause the system to recognize the holes. 4
7. Select Workpiece from the Search Method list. 8. Click Find Features. 9. Click OK in the Find Features dialog box. 10. Click in the background of the Machining Feature Navigator to deselect the features. 11. In the background of the Machining Features Navigator, MB3 Group Features. This option allows you to group features based on the feature type. The first feature groups you will create will be for thread features. 12. In the Features to Group section of the dialog box, be sure All Features is selected from the Method list. This will list all features in the Feature Types list. 13. Using the Ctrl key, select the three thread feature types. 14. Click Identical Attributes to clear the box. When turned on, this option causes each group to contain features with identical attributes (i.e. diameter, depth). You will use this option when creating feature groups for hole features. 15. Click Create Feature Groups. 5
The Feature Groups list allows you verify the groups you wish to create before finalizing the group creation. If you select an item in the Feature Groups list, the geometry will highlight. You may remove groups from the list by clicking the Delete button. 16. In the Feature Groups section of the dialog box, select any of the feature groups to highlight the geometry in the graphics window. The next feature groups you will create will be for hole features. 17. Select STEP2HOLE in the Feature Types list. 18. Click Create Feature Groups. 19. Select STEP1HOLE in the Feature Types list. 20. Click Identical Attributes. Each group will contain features with identical attributes (i.e. diameter, depth). 21. Click Create Feature Groups. 22. Click OK to complete the creation of the feature groups. 23. Display the Geometry View of the Operation Navigator. 6
Create a Manual Spot Drilling Operation You will use the feature groups to create manual drilling operations. 1. Select the FG_STEP2HOLE_THREAD feature group. Notice the geometry that highlights. 2. MB3 on FG_STEP2HOLE_THREAD and click Insert Operation. 3. Select hole-making from the Type list. The first four operation subtypes are new for holemaking. 4. Select SPOT_DRILLING. 5. Specify the following: Program: Tool: Geometry: Method: NC_PROGRAM UGT0321_009 FG_STEP2HOLE_THREAD METHOD 6. Click OK. 7. Click Display next to Specify Hole or Boss. 7
The in-process feature volume for the geometry group is highlighted. 8. Click Generate. 9. Click OK to complete the spot drilling operation. Create a Manual Drilling Operation 1. Select the FG_STEP2HOLE_THREAD feature group. 2. MB3 Insert Operation. 3. Select DRILLING. This operation subtype is used for drilling, reaming, and boring. 4. Specify the following: Program: Tool: Geometry: Method: NC_PROGRAM UGT0301_039 FG_STEP2HOLE_THREAD METHOD 5. Click OK. 6. Click Display next to Specify Hole or Boss. 8
The in-process feature volume for the geometry group is highlighted. Notice that it does not reflect the full depth of the hole you wish to drill. 7. Click Specify Hole or Boss. 8. Select FACES_CYLINDER_2 from the Machining Area list. Notice that the in-process feature volume changes. This machining area will allow the operation to drill to the full depth of the hole. 9. Click OK. 10. Click Generate. 11. Click OK to complete the drilling operation. 9
Create a Hole Milling Operation 1. Select the FG_STEP2HOLE_THREAD feature group. 2. MB3 Insert Operation. 3. Select Hole Milling. 4. Specify the following: Program: Tool: Geometry: Method: NC_PROGRAM UGT0201_103 FG_STEP2HOLE_THREAD METHOD 5. Click OK. 6. Click Display next to Specify Hole or Boss. The in-process feature volume for the geometry group is highlighted. 7. Click Generate. 8. Click OK to complete the hole milling operation. Create a Thread Milling Operation 1. Select the FG_STEP2HOLE_THREAD feature group. 2. MB3 Insert Operation. 3. Select Thread Milling. 10
4. Specify the following: Program: Tool: Geometry: Method: NC_PROGRAM UGT0231_005 FG_STEP2HOLE_THREAD METHOD 5. Click OK. 6. Click Display next to Specify Hole or Boss. The in-process feature volume for the geometry group is highlighted. This is not the machining area you wish to thread. 7. Click Specify Hole or Boss. 8. Select FACES_CYLINDER_2 from the Machining Area list. Notice that the in-process feature volume changes. This machining area you wish to thread. 9. Click OK. 11
10. Click Generate. 11. Click OK to complete the thread milling operation. 12. Close the part without saving. Open drilling_example_with_operations.prt and explore some of the operations that have been created. When you have finished, close the part file without saving. 12
Siemens Industry Software Headquarters Granite Park One 5800 Granite Parkway Suite 600 Plano, TX 75024 USA +1 972 987 3000 Americas Granite Park One 5800 Granite Parkway Suite 600 Plano, TX 75024 USA +1 314 264 8499 Europe Stephenson House Sir William Siemens Square Frimley, Camberley Surrey, GU16 8QD +44 (0) 1276 413200 Asia-Pacific Suites 4301-4302, 43/F AIA Kowloon Tower, Landmark East 100 How Ming Street Kwun Tong, Kowloon Hong Kong +852 2230 3308 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 www.siemens.com/plm. 2013 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. 8/13 www.siemens.com/plm/nxmanufacturingforum 13