PTC Technical Specialists E-Newsletter Date: December 1, 2006

Transcription

1 PTC Technical Specialists E-Newsletter Date: December 1, 2006 PTC Product Focus: A) What s New in Sheetmetal Design for Wildfire 3.0 B) Windchill 3 rd Party Workgroup Managers Tips of the Month: A) Creating Sheetmetal Drawings in Wildfire 3.0 Announcements: Most Recent Announcements B) Mapping a CATIA V5 Parameter to a Windchill Attribute Upcoming Events & Training Schedule: Events & Training Schedule PTC Product Focus What s New in Sheetmetal Design for Wildfire 3.0 With Pro/ENGINEER Sheetmetal Design, PTC has enhanced the speed and flexibility with which sheetmetal part creation takes place. New user interfaces allow for the quick creation of flat and flanged walls of all shapes and sizes. Complex sheetmetal parts with multiple overlapping surfaces can be created with automatic miter cuts, saving valuable time in the design process. Using the Flange Tool to Create Multiple Walls The Flange Tool (Click Insert > Sheetmetal Walls > Flange or the flange wall icon ) allows for the creation of flange wall features along tangent and non-tangent edges. This is particularly useful for creating multiple identical sheetmetal walls along the edges of a base surface. Wall segments can be included and excluded as needed providing ultimate flexibility in the rapid creation of enclosed sheetmetal parts. Customer PTC E-Newsletter 12/1/2006 Page 1 of 22

2 Sheetmetal enclosure containing 4 identical walls The corner relief is also defined during the creation of multiple walls. Each relief can be updated through navigation in the dashboard (Click Edge Treatment), providing further design flexibility during sheetmetal part creation. Define the relief for each corner individually, or all at once. Corner relief using the dashboard user interface Customer PTC E-Newsletter 12/1/2006 Page 2 of 22

3 Speed up the design process by taking advantage of automatic miter cuts. Create intersecting sheetmetal walls without the hassles of material overlap. Define automatic miter cuts using the dashboard user interface New Sheetmetal Cut User Interface Adjust material removal properties to drive sheetmetal design processes. With the ability to define material removal normal to both the driving and driven surfaces, components placed at angles will not cause interference in the assembly. Customer PTC E-Newsletter 12/1/2006 Page 3 of 22

4 Material removal normal to driving surface Material removal normal to driven surface Customer PTC E-Newsletter 12/1/2006 Page 4 of 22

5 Material removal normal to both driving and driven surfaces New Unattached Extruded Wall User Interface With the unattached extruded wall user interface, it is possible to create complex sheetmetal parts in very little time. Simply create a profile sketch and use the dashboard to define the sheetmetal characteristics such as bend radii and thickness. By creating unattached extruded walls, multiple wall creation steps can be combined into one operation. Customer PTC E-Newsletter 12/1/2006 Page 5 of 22

6 Base sketch in sketcher mode Resulting sheetmetal part as specified using the dashboard user interface Customer PTC E-Newsletter 12/1/2006 Page 6 of 22

7 Sheetmetal Reports By using the embedded web browser in Pro/ENGINEER, access to critical design information is available (Click Info > Model). Browse information about the sheetmetal part such as bend allowances, bend radii, and Y and K factors. Selecting individual feature information items in the web browser will result in automatically highlighted features in the Pro/ENGINEER working environment, adding clarity to the available information. Sample sheetmetal information report using Pro/ENGINEER s embedded web browser More Information on Sheetmetal Design To find out more about Pro/ENGINEER s Sheetmetal Design visit our Website. Back To Top PTC Product Focus Windchill 3 rd Party Workgroup Managers Click Here To View Back To Top Customer PTC E-Newsletter 12/1/2006 Page 7 of 22

8 Tips of the Month Creating Sheetmetal Drawings in Wildfire 3.0 With Pro/Engineer Wildfire 3.0 comes the introduction of shaded drawing views. These drawing views are also available with sheetmetal design. In the following pages, we will walk through the process of creating a simple sheetmetal drawing with both the finished manufactured part and its flat state instance. We will touch on creating flat patterns as well as bend order tables. To begin, we will start with a sheetmetal part that has already been designed and then create its associated flat state instance. This can be achieved by clicking Edit > Setup > Sheetmetal > Flat State > Create. Creating the flat state instance Accept, or rename, the flat state instance, and then select the unbend operation. From this point, all the user needs to do, is select the surface to remain fixed during the unbend operation. Customer PTC E-Newsletter 12/1/2006 Page 8 of 22

9 Selecting fixed surface geometry Finally, click OK to complete the feature. The flat state instance is now displayed in a new Pro/ENGINEER window. Flat state instance Notice that the flat state instance and name are displayed in the Pro/ENGINEER graphics window. From this point, the flat state instance window can be closed. You can check the instances for the generic part by clicking Tools > Family Table. Customer PTC E-Newsletter 12/1/2006 Page 9 of 22

10 Family Table for sheetmetal part Having created the flat state instance, attention can now be focused on the manufacturing aspect of the part. In particular, we will take a look at creating the bend order sequence. This is also achieved by clicking Edit > Setup from the main menu, followed by Sheetmetal > Bend Order > Show/Edit from the Menu Manager. Selecting the same fixed surface as before (when creating the flat state) returns the sheetmetal part to its flat state. Click Add Bend to begin creating the bend order sequence. Customer PTC E-Newsletter 12/1/2006 Page 10 of 22

11 Creating the bend order sequence Select the first feature for the bend order sequence and click OK. Customer PTC E-Newsletter 12/1/2006 Page 11 of 22

12 Selecting first bend feature Click Next and select the fixed surface (the same surface used to create the flat state). Beginning second bend feature After selecting the fixed surface, hold the CTRL key and select the remaining bend locations. Customer PTC E-Newsletter 12/1/2006 Page 12 of 22

13 Selecting multiple bend locations Click OK > Done to finish creating the bend order sequence. The part returns to its finished state. Finished bend order sequence Customer PTC E-Newsletter 12/1/2006 Page 13 of 22

14 Clicking Info from the Bend Oder menu displays the information for the bend order sequence. Bend Oder Sequence Information Window Now that the flat state and bend order sequence have been created, it is time to create the sheetmetal drawing. Click New from the main toolbar to create a new drawing (set type to Drawing). Clear the Use default template check box and click OK. Make sure that the Default Model for the drawing is the correct sheetmetal part and click OK. Customer PTC E-Newsletter 12/1/2006 Page 14 of 22

15 Drawing setup When prompted, select the generic instance for the model. Right-click to insert a general view. Click in the upper right-hand corner of the drawing window to place the view. Select OK from the Drawing View dialogue box to complete view placement. Right-click and select Lock View Movement to enable repositioning of the drawing view. Reposition and rescale the view as necessary. Placement of first drawing view Customer PTC E-Newsletter 12/1/2006 Page 15 of 22

16 Now we can add the flat state instance to the drawing. Select File > Properties from the main menu. Click Drawing Models > Add Model to add the flat state instance. Select the sheetmetal part and click Open. Select the flat state instance from the menu and click Open. The active model will switch from the generic to the flat state instance. Click Done/Return. Create a drawing view of the flat state instance in the same fashion as the shaded model. Right-click and select Insert General View. Click anywhere in the drawing window to place the view. Use the View Display dialogue box to adjust the view display settings. Once finished, click OK. Placement of second drawing view To finalize the drawing, we will add bend lines and the bend table. Select the Show/Erase icon. Click Show and select the options for Notes and Axes to be displayed. Click Show All > Yes to display the notes in the view. Click Accept All. Customer PTC E-Newsletter 12/1/2006 Page 16 of 22

17 Show / Erase dialogue box Click Erase > View and select the shaded view to remove the bend information from that view. Select Close from the Show / Erase dialogue box to complete the drawing. Customer PTC E-Newsletter 12/1/2006 Page 17 of 22

18 Final Drawing Notice the bend table in the upper left-hand corner. Also note the bend axes and angles in the left-hand view. That completes the drawing. So by using both new sheetmetal and drawing enhancements in Pro/ENGINEER Wildfire 3.0, users can create detailed drawings for sheetmetal parts with relevant manufacturing information and shaded 3D drawing views. Back To Top Tips of the Month Mapping a CATIA V5 Parameter to a Windchill Attribute Click Here To View Back To Top Customer PTC E-Newsletter 12/1/2006 Page 18 of 22

19 Announcements Educational Resource Library Learn things you always wanted to do - but didn't know you could. This one stop educational resource library will help you learn more about PTC Solutions and provide you with technical materials developed by the product experts to help you become more productive. Get tutorials, how-to videos and expert advice for: Pro/ENGINEER Conceptual and Industrial Design Detailed Design Simulation/Analysis Production Design Collaboration Windchill PDMLink Windchill ProjectLink Pro/INTRALINK PTC Online Tools Check out the Educational Resource Library today. PTC Tips & Techniques Newsletter Archives Miss an issue! Can t find that awesome technique you read about? Fear not, you can click on the link below and go through our Customer PTC E-Newsletter archives. It s better than finding the Covenant of the Ark! Click Here To Access PTC Tips & Techniques Webcasts: Work Smarter. Not Harder. Click below to see regularly scheduled Tips & Techniques technical Webcasts that are designed to provide you with the most popular time-saving tricks that Pro/ENGINEER users of all skill levels will find useful. Get more out of your maintenance dollars! Tips & Techniques: Work Smarter Not Harder! E-PROFILES IS HERE!! We have been eagerly anticipating the debut of the new electronic version of Profiles Magazine and now it is here! This new web site will supplement the print edition of the magazine and will Customer PTC E-Newsletter 12/1/2006 Page 19 of 22

20 provide new useful features not feasible with paper media. e-profiles will provide you with 24x7, worldwide access to key information previously available exclusively in the print version. "Tips & Tricks," a popular feature pioneered by Pro/USER, has also moved to the web and will be expanded as the site matures. Please take a few minutes to check out this new web site. We don't think you will be disappointed. Back To Top Customer PTC E-Newsletter 12/1/2006 Page 20 of 22

21 Upcoming Events & Training Class Schedules Upcoming, 2006 June 3-6, 2007 Your local Pro/Engineer User Groups Tampa, Florida PTC/USER International Conference Events Our seminars and conferences seek to provide you with relevant information regarding product development trends in your industry as well as innovative software learning experiences. Think of them as a constructive day off where you can share experiences and swap ideas with your peers. If you can't manage to get away, we'll bring it to you. Check back often for regularly scheduled live webcast events. You re Invited to Attend Please visit the PTC Education Services website for the latest training information including course descriptions, schedules, locations, and pricing. Attend a course at any PTC Center and receive a free copy of Pro/ENGINEER Wildfire Student Edition! Live Instructor-Lead Virtual PTC Training Courses Virtual Classrooms provide interactive learning with a trained PTC instructor in convenient and manageable sessions that last approximately 4 hours over a series of days. It's easy to join a class right from your desk using a phone or voice-over IP technology. Sessions are performed just like a traditional ILT (including interactive exercises where you and the instructor can work on lab exercises together) and feature some of our most popular ILT courses. These sessions cover the exact same material as the traditional ILT in-center courses. Also look for some of our most frequently requested mini-topics delivered in the same format that are only an hour - two hours in duration. If you have any questions about these sessions or would like to see getting other courses, not on this list, on the schedule please feel free to contact me for more details. They are a great way to bring training to you without you having to worry about location or being out from work for long stretches. Customer PTC E-Newsletter 12/1/2006 Page 21 of 22

22 You can register for these sessions just as you would for any normal ILT class either by: 1. calling order admin at or 2. you can go to PTC University directly at and submit a registration request directly. All you have to do is search the catalog by typing in virtual in the search field and you will see a listing. PTC Note: This PTC E-Newsletter will continue to be used for the following: 1) Inform you on events related to PTC products (user groups, conferences, training schedules, etc.) 2) Educate you on solutions that are available at PTC 3) Tips & Techniques using PTC Products Note: These messages are compiled in the local PTC office and will be distributed via . Back To Top Customer PTC E-Newsletter 12/1/2006 Page 22 of 22