Spring 2004

Jason Clark explains why "reverse engineering" your Pro/ E model is a key concept for applying the top-down design philosophy.

"Reverse Engineering" Your Pro/ENGINEER Models for Top-Down Design by Jason Clark

Dynamic Publishing Technology Supercharges PTC/USER Web Site by Rick Snider

Creating a Parametric Note Block by Kenneth S. Johnson, ITT Industries Using Relations to Assign Different Materials and Mass Properties for Family Table Instances by Dwaraka Nadha Reddy of Motor Control Centers, GE-IBC

Making Progress on PTC Software Enhancements by Evan Caille Discover Your Future In Nashville by Rick Snider

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Why would you want to “reverse engineer” your Pro/ENGINEER model? Simply because the first model you make isn’t the final one. After all, there’s always something to tweak whether it be for clearance, machining allowance or some other refinement. The process of adding top-down design functionality to existing models is actually part of the top-down design (TDD) process. Quite often you will brainstorm an idea with little or no constraints. Once you are happy with the overall concept, you will then add intelligence to the model by implementing the TDD functionality. You can’t think of all the variables at the start of the design, so you take an educated guess and progress. The idea of reverse engineering your models is to apply what you learn through the design phase to add intelligence to your models for final production.

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When people ask why develop models that adhere to the TDD philosophy, the easiest answer is “because Pro/ENGINEER is designed for it.” In truth, Pro/ ENGINEER has very powerful tools to administer and control your designs. Utilizing TDD practices offers many advantages including the ability to: ●

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Administer changes to many models from just one “document” (called a layout) Control the flow of changes, and the effect of the changes, over many models Rough out designs and create concepts without designing any detailed parts Easily generate spin-offs from an existing design Empower your Pro/ENGINEER assemblies to adapt to change, including part replacement.

Our Objective The example used throughout this article is a hydraulic/pneumatic cylinder that begins as a typical Pro/ENGINEER assembly and is reverse-engineered to leverage the TDD principles (see Figures 1 and 2). By “typical” assembly, I am referring to the bottom-up approach in which a Pro/ENGINEER user models each piece of an assembly and manually compares values to ensure their validity. Models of this type contain minimal intelligence and thus do not automatically adjust to dimensional changes or even model replacement.

Figure 1. Exploded assembly

Figure 2: Assembly model tree After reading this article, you should be able to add TDD features in one form or another to enhance legacy Pro/ENGINEER models. The following discussion assumes you have a fairly good understanding of the Pro/ENGINEER software interface, as well as a basic concept of what TDD is and how it functions within Pro/ENGINEER. 1. Start with a Blueprint Before we progress too far, we need to ask a few questions to ensure we attain the goals we want our Pro/ENGINEER model to achieve. Applying TDD does

require some forethought and planning. I say this because once you start, you can get carried away and create too many parametric links. This makes your models hard to work with in the future—especially if you do not document them carefully. Even though top-down design does take upfront effort, you will find that as you develop best practices applying TDD will become second nature. If you ever have to modify a TDD drastically, you will find that you can complete changes faster than if you were working with an assembly with no TDD methodology. So let’s create some assumptions and goals for our cylinder assembly. It must be able to: a. Adapt to the piston bore size. b. Adapt with a change in stroke length. c. Adapt with a change in shaft diameter. Albeit a small step for this particular exercise, this kind of planning is crucial for any design you try to accomplish in Pro/ENGINEER. 2. Sherlock Time! Now assume we have no prior knowledge of the Pro/ENGINEER models we are to work with. Perhaps you are a contractor continuing someone else’s design or perhaps you are tweaking your model for production. Since we are dealing with an existing design, a lot of work has already been done and we do not want to contradict the design intent. The easiest way to learn the assembly intent is to browse the assembly and its components to make note of constraints. Investigate the assembly and become familiar with it. Later in the process, the goal will be to reroute the assembly constraints to a skeleton. Browse the constraints in Figures 3-6 using Info_Component:

Figure 3.

Figure 4.

Figure 5.

Figure 6.

3. Lay It Out! At this point, we know what our goals are for controlling the assembly and have determined the method of assembly for each component. The next step is to document the master plan—often a weakness in parametric modeling. Documentation is the key with TDD since it is almost as powerful as actually

implementing the parameters and relations to control the design. To document the intent of the design, we use a layout. A layout is a twodimensional representation of our design that may contain static sketches and tables containing parameter data. While sketch data can be made within layout mode, I recommend importing 2D views whenever possible. Sketching in Pro/ ENGINEER’s layout mode is weak and can be time-consuming. If you are dealing with a design that is already documented, export the drawing as an iges file and import it into your layout. Once you have imported the data, you can delete what is not needed. Other options are to import dxf, dwg and Pro/ ENGINEER overlays. (Imported iges, dxf, and dwg data can be edited within layout, but Pro/ENGINEER overlays cannot.) Figure 7 shows our layout, which is an imported IGES file (from an existing drawing). Refer to the notes below the figure.

Figure 7. Layout view (click to enlarge) Bear in mind there are many ways to go about controlling a design, and what I have illustrated here is a simplified interpretation. What you see in the layout is a sketch and enough dimensions so that we can control the key aspects of the cylinder. By creating a dimension in layout (Edit_Insert Dimension), you in fact create a parameter because, when prompted, you need to enter a parameter name and give a value Once the dimensions are done, I recommend creating a table using a repeat region. For our example, I created a two-column table and used the report parameters lay.param.name and lay.param.value in the repeat region. I then added a filter to show only layout design parameters (i.e., the LY_ prefixed ones).

Now it’s time to add relations. For now, the parameter LY_PISTON_STROKE is controlled by a relation LY_PISTON_STROKE=LY_GLAND_STRK – LY_PISTON_THK. Alternatively, you could write a relation to control the stroke with LY_PISTON_STROKE value and a relation would update LY_GLAND_STRK and LY_PISTON_THK. There are many ways to go about this, and ultimately the choice is yours. The important areas of a layout are: ●

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Parameters to contain numerical data or textual data (e.g., notes, specifications) Relations to create intelligence and to generate rules for the dimensions (e. g., shaft_bore=
A few key things about layouts to keep in mind: a. The sketches are not parametric and are best imported from an existing file such as dwg, dxf or iges. I recommend the import if you’ve done some preliminary sketching (e.g., using AutoCAD), or the export of detail drawings you’ve done using the iges format. The sketching tools in layout are weak, but you can get by with them if necessary. b. Naming convention is a definite consideration that requires some thought. I suggest: ■ Prefixing layout parameter names so they are easy to distinguish in your parts and assemblies. This practice protects you from parameter conflicts upon declaring your layout. These conflicts generally happen when you use a PDM tool like Pro/INTRALINK or if you use generic names that may appear in parts. You need to be careful here because you can overwrite parameters in parts and assemblies that have the same name in a layout. ■ Defining your datum name scheme since the names will be used throughout your parts and assemblies. c. Add datums to your layout (Edit_Draft Datums). This step is very important because it documents the design assembly constraint intent and allows you to use layouts to drive automatic component replacement if desired. 4. Skeletons Out of the Closet For TDD, skeletons are a fabulous—and essential—tool. Skeletons are the threedimensional representations of our layouts. The links from layouts to skeletons are the parameters, relations and datums we define in the layout. For visual purposes, I find it handy to add surface geometry. To illustrate, imagine a large assembly. Adding surfaces can be a lifesaver because you can define work area boundaries that represent a physical volume of a subassembly (for example, a surfaced rectangle could represent a drivetrain). The surfaced rectangle acts as the physical boundary of a subassembly and provides a visual indicator for other designers to recognize items that infringe on the boundary. This helps to resolve interferences immediately. To prepare the skeleton, open the assembly and select Component_Create_Skeleton from the side menu. You should specify a start part if you utilize start parts (i.e., templates). Be sure to name the skeleton _SKEL. Once your skeleton is defined in the assembly, save the assembly and open the skeleton in a new window.

The next step is to lay down your foundation. In Figure 8, note the naming of the datums since those datums within the layout will need to be represented within the skeleton. I recommend labeling key skeleton datums with a prefix (in this case, SK_). Naming datums and prefixing them can be invaluable when you have many datums. Naming datums also helps when using Sel by Menu operations. Feel free to add motion controllers, such as the datum SK_MOVE_PISTON. We will add a relation to limit movement of SK_MOVE_PISTON based on values in our layout.

Figure 8. (click to enlarge) To fill things in a bit, add some surface geometry to help with visualization. Note in Figure 9 that the piston is roughed in.

Figure 9. (click to enlarge) Now that we have geometry, we need to associate the values from layout to skeleton. First off, we have to declare the layout to our skeleton. Open the layout created earlier into session and then activate the skeleton window. Select Set Up_Declare_Declare Lay and then select the layout name from the menu. You can only declare layouts that are in session. Open up your relation window and add the relations to control the skeleton’s geometry. Adding relations depends heavily on the design intent and is one tool to capture that intent. Be sure to comment your relations! (See Figure 10 for an example.)

Figure 10. At this point, we can use the skeleton to look at how the geometry can be manipulated and in doing so we can do case studies, test geometry movement, etc. For example, modify the datum SK_MOVE_PISTON and give it a value like 20. Regenerate the model and see what happens. Putting It All Together Let’s open up our assembly that contains our super-smart skeleton.

Figure 11. (click to enlarge) But as you can see in Figure 11, it’s quite a mess. At this point, you may wonder what we’ve accomplished. Without linking in the skeleton, we probably have not gained a whole lot. Once we link our parts to the skeleton, though, we will have a very robust assembly. Looking at our sample cylinder, what would happen if we deleted the cylinder tube? Pretty obvious, we’d be in resolve mode because our parent-child relationships would blow up. A skeleton (or skeletons) is the way to prevent this bomb. Skeletons always reside at the beginning of the model tree. By adding skeleton(s) to our assembly, we have a stable foundation on which to build our parts. The goal is to logically associate as many items to a skeleton so that no one part or subassembly can create havoc if removed. The objective of skeletons is to maintain integrity and assembly constraints for the components we’re designing, and we would not typically create datum geometry for fasteners and generic hardware. With the assembly open, redefine each component to the skeleton using the appropriate references. If you are not sure which datums to use, refer to the layout. I hope things are starting to click now!

Figure 12. (click to enlarge) What is going on here? In Figure 12, I redefined the components to match the constraints defined in my layout so it should look like my layout! Well, not quite. The last step is to pass intelligence to the parts that make up the assembly. We can now either use copy geometry from the skeleton to define boundaries and use those features to fix the parts, or we can apply our layout to the parts. I will illustrate the second approach. Using copy geometry is a quick fix, but it will build a dependency to the assembly. If your assembly is large, making a change that results in a copy geometry feature requiring regeneration means you have to load the entire assembly into session to complete the regeneration. Declaring a layout to our parts eliminates this step. By using a layout, you can work on a part with only it and a layout open in session, saving all that regeneration time for other things! For example, to fix the short cylinder tube, we can modify the tube to contain the extra dimensional information and add a relation to keep things in order. When complete, our cylinder should look like Figure 13.

Figure 13. (click to enlarge) To accomplish the geometry, I declared the layout (Declare_Declare Lay, in part mode) and added the following relations (Figure 14).

Figure 14. I then modified the piston part by declaring the layout and adding some relations to ensure clearances (Figure 15).

Figure 15. Just to confirm we’re going in the right direction, we can compare our cylinder to our skeleton with a simple shade test. The blue and yellow represent the cylinder tube and piston in the skeleton. As you can see, we have a perfect fit (Figure 16).

Figure 16. (click to enlarge) From here, you can declare the layout to the other parts and associate the values from the layout to their respective dimensions in each part. Once we have completed the associations, we then fulfill our plan to: a. Adapt to bore size. By varying the LY_WALL_THK parameter, we can change the cylinder internal bore, which in turn automatically adjusts the piston diameter. b. Adapt to stroke length change. By varying the LY_GLAND_STRK parameter, we can lengthen the cylinder, which in turn automatically updates the parts placement since the skeleton will update its datum offsets. If we were smart, we would have added a relation to our piston part to associate its length to the stroke. c. Adapt to shaft diameter. By varying the LY_SHAFT_DIA parameter, we can adapt the shaft end gland bore to accommodate a shaft size change. Conclusion I have covered a lot of basics to help you start to integrate some top-down design methodologies into your older models. By taking two simple steps with a layout and a skeleton, you almost immediately add greater control and stability to your Pro/ENGINEER assemblies. Many other tools complement the top-down design methodology—such as copy geometry, replace by layout, shrinkwraps and envelopes—but are outside the scope of this article. I encourage you to review these and other options for leveraging all that Pro/ENGINEER has to offer.

Jason Clark is a senior designer and PTC application administrator at OceanWorks International. Jason also chairs the Vancouver PTC/USER group. He can be reached by e-mail at [email protected].

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The Internet plays a vital role in sustaining the PTC/USER community. Although our membership is spread across six continents and works in a multitude of industries, electronic communications help us transcend the enormous geographical distances to exchange information, solve problems, and improve productivity. After a thorough reevaluation of our network infrastructure in early 2003, it was clear that further investment was required to provide PTC/USER members with the capabilities appropriate for a leading-edge organization. As a result of this project, we are pleased to introduce the next evolution of our Internet services. Our new web site or portal, members.ptcuser.org, integrates many existing technologies to create a powerful means for memberto-member interaction. Here are some of the important new capabilities that members.ptcuser.org now offers. ●

Database publishing. Thanks to new relational database technology, the PTC/USER web site now dynamically updates member information. This critical upgrade serves to move the power to publish out of the hands of a privileged few and extends it across the entire PTC/USER community. Individuals can now revise event and group information instantly, giving all community members timely access to news. In addition, we have centralized and consolidated our member database, replacing multiple redundant, obsolete, inaccessible and frequently inaccurate systems. With this change, individuals have complete control over access to their contact information. For example, Technical Committee members may choose to let other committee members see their mailing addresses and phone numbers, but only make their e-mail addresses available to the wider community. Members can even block all access to their contact information, if desired.

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PTC/USER has a long tradition of staying at the forefront of Internet technologies. Don Patterson initiated our first communication service, the e-mail exploder, back in 1991, and shortly thereafter followed up with an FTP site for file sharing. Our initial web site debuted in 1994—well before most of the world (including PTC) established a presence in this wild, wide-open frontier. For those of you who are curious to see how ptcuser.org has evolved over time, you can consult the Wayback Machine, a vast historical archive of the Internet located at web.archive.org.

Communications. For our e-mail exploders, the site now uses Lyris 7.0—a major upgrade of our mailing list management software. Online

chat rooms are a new feature, where members can now participate in realtime discussions of Pro/ENGINEER®, Pro/INTRALINK®, Windchill® and other PTC software-related issues. ●

Collaboration. PTC/USER Technical Committees and Regional User Groups now have the benefit of enhanced collaboration services. Through document management services, TCs and RUGs can disseminate important information to their members, as well as establish workflows for in-process documents such as white papers. They can also schedule events on the PTC/USER master calendar, manage member registration for their groups, and conduct online surveys to gather feedback. Each group and committee also controls its own web site home page and can edit the information using a forms-based tool rather than HTML.

A sample screen from the new members web site.

During phase two of this project, we will add other advanced features that build

upon this new foundation. Some potential areas for expansion include an online knowledge base, overhaul of the discussion system, and training services. We welcome your feedback and suggestions for other improvements you would like to see at members.ptcuser.org. Though much has changed over the years, one thing that’s still the same is the price. PTC/USER membership remains free of charge, thanks to the support of members and our Industry Partners for activities such as the PTC/USER World Event. It’s hard to imagine any free service today that can make such a different in your day-to-day work, let alone one that has the extensive resources offered by ptcuser.org. If you haven’t registered as a member, you’re really losing out, so don’t wait—join PTC/USER today. We hope to see you online soon. Rick Snider is Executive Director of PTC/USER and is also the webmaster for the ptcuser.org site. He can be reached at [email protected].

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Nearly 110 PTC/USER Technical Committee members braved the New England cold to gather at PTC’s headquarters in Needham, Massachusetts for three days in January. Thirteen TCs conducted onsite meetings, drawing participants from North and South America, Europe, and Japan. During the sessions, TC members met with PTC product managers to review current and future software development projects. Two common themes that recurred throughout the discussions were PTC’s new enhancement database and the increasing importance of the Product Development System Technology Roadmap to the company’s software planning process. Setting the Stage A week before the Massachusetts meetings, Brian Shepherd, PTC’s Senior Vice President of Product Management, conducted a webcast for TC members on PTC’s current corporate and product strategy. Shepherd described how PTC is evolving its Product Development System Technology Roadmap, a guide for developing solutions that address specific business processes. He also spoke about the increased integration between the MCAD and Windchill products, and reconfirmed PTC’s commitment to future product development and technical support. In addition to the PTC executive overview, a number of the Technical Committees also held webcasts in advance of the meetings. TC members benefit greatly from these preliminary discussions so that they all share the same baseline information before the face-to-face sessions. PTC/USER hosted an evening reception for TC members and PTC’s product management organization. This informal get-together provided another valuable opportunity for meeting attendees to network and exchange information. Based on the amount of interaction, this event was a great success. New Enhancement Database During the TC chairs’ dinner, PTC demonstrated a simulated design process highlighting the integration of Pro/ENGINEER, PDMLink, and ProjectLink. PTC also explained its new enhancement process and how it will affect TC discussions. TC members agree that the new process is a positive step toward including the needs of all users in product planning activities. In particular, the enhancement process now provides much needed organization and a feedback loop for requests. Individuals who submit enhancement requests will receive a reply from the appropriate PTC product manager about the status of those requests. In addition, product managers will be able to extract a report of enhancement requests pertaining to the products covered by a particular TC.

This will enable TC members to consider enhancements during the specification and prioritization process. The link to the new enhancement request form can be found on PTC’s Technical Support page at www.ptc.com/support/ support.htm. Session Highlights Several of the Technical Committees that met in January provided the following summaries of their sessions, including their current focus of activity. Core Modeling drew members from Europe, North and South America, as well as visitors from several other TCs. The discussions centered on product development plans and projects related to finishing or extending functionality introduced in post-Wildfire releases of Pro/ENGINEER. The TC met to prioritize their white paper efforts and review PTC projects currently under development. Topics under consideration include: ●

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config.win. May be co-developed with the System Administration TC. Mirror of Part, Assembly, Drawing, and Instance. Would expand on a paper developed by the Sheet Metal TC Model Compare Functionality. Relates to a series of TC white papers addressing design data change and change management.

Netesh Gohil and Ric Leeds of PTC led a use case development session on several projects, including Resolve Mode, Annotation Features, Sketcher Tools, and View Manager. Dan Glenn of Solar Turbines described the implementation of Wildfire at his site. Heinrich Bartels of Stewart and Stevenson Services presented his work regarding development of a user interface for generating and managing corporate model/drawing notes. Customization met with eight TC members and three PTC representatives. The sessions featured an interesting user presentation on software revision using a product called Concurrent Versions System (CVS). PTC presented enhancements and improvements for upcoming releases, plus a tutorial on customizing the Wildfire user interface. Interest in J-Link programming seems to be increasing. Data Exchange and Archiving had 10 attendees. The group reviewed enhancements to Wildfire 2.0 and discussed potential improvements in Wildfire 3.0. The TC will complete two white

Changes in TC Leadership As a volunteer organization, PTC/ USER relies on its members to provide leadership. While serving as a Technical Committee chair is a rewarding experience, it is also a timeconsuming commitment. As a result, committee chairs are often forced to step down if they have to take on new responsibilities at work or if their companies are in a major transition. That is the case for several committee chairs at this time. I would like to thank the following individuals for their dedicated service to the TC process. I know that their committee members share in this appreciation. Ben Franklin, Data Management Jonathan Durston, Sheet Metal Jeff Bradley, Data Exchange and Archiving Rick Yahn, Windchill Solutions Kristine Bothwell, Visualization Karen Dougherty, Usability and Training I also want to welcome following individuals who have now taken up leadership of these

papers and conduct a survey before the June meeting. Members have agreed to meet via webcast every six weeks to comment on enhancements before they go into the software. Data Management has conducted webcasts throughout the year. The January meeting was well attended by member companies and PTC product management. Areas of discussion include change management, archiving, migration, maturity states, and product roadmaps for PDS, Pro/INTRALINK, and Windchill. Several webcasts are planned over the next couple of months to further support these efforts.

committees. Mark Crum, Data Management (Acting Chair) Joel Nelson, Sheet Metal Matt Meadows, Data Exchange and Archiving Jeff Zemsky, Windchill Solutions

Industrial Design and Surfacing conducted inJill Schwegel, depth discussions on Style, Re-Style, Global Visualization Modeling (Warp) and Photorender within Wildfire 2.0 and 3.0. Enhancements to the recently released Pro/CONCEPT conceptual design software Denise Justice, were also covered. Among the highlights of the Usability and Training meeting was an announcement that Pro/CONCEPT 2.0 will open native Pro/ENGINEER files when run in a Windows environment. In addition, PTC described various enhancements to the Style, Re-style and Global Modeling features that the TC was instrumental in identifying. Product Development System, our newest TC, has a unique focus and structure. Rather than software functionality, the PDS committee concentrates on specifying the business processes that companies use to develop products. The TC helps give PTC a better understanding of the different ways companies approach the development process. The PDS committee is made up of members of the other TCs in order to bring a broad perspective to the discussion. The goal is to review each process on roughly a two-month schedule, resulting in a process guide that can be used with the Product First Roadmap. Our first topic is change management and the team has already started giving PTC feedback in this area. The second topic will be top-down design. Routed Systems discussed future enhancements, bug reports, and customizations of Routed Systems Designer, Pro/CABLING, Pro/HARNESSManufacturing, Pro/PIPING and Pro/ECAD. The meeting was a great success, generating many new ideas that were recorded by the product manager and software developers (some of whom teleconferenced in from as far away as Israel). The Routed Systems Technical Committee is focused on providing input to PTC in such areas as government contracts, industrial plumbing, semiconductor, and aerospace. Sheet Metal discussed a number of key issues including top-down design in sheet metal, sheet metal materials, simplifying wall creation methods, form placement and UDFs. In the coming months, the TC will finalize several white papers including those on mirror functionality and sheet metal reports. Members will conduct conference calls on new projects in development for Wildfire 3.0. Our focus is on future releases of the sheet metal module and their impact on the user community. Usability and Training discussed areas of training and proficiency and ModelCHECK. CADTRAIN continues to add new course offerings, including Pro/ MECHANICA Structure, Pro/INTRALINK 3.3 and Wildfire. Coach content is AICC-

compliant, allowing plug-and-play with other LMS systems. PTC has also launched a new program called PTC University, built on the LMS concept, which brings together all areas associated with learning, from searching for learning opportunities to tracking enrollments to accessing role-based communities. Discussions continued about ModelCHECK’s increased checking functionality and user interface enhancements. The committee also discussed PTC’s adoption aids for Wildfire 2.0. Visualization discussed licensing, new ProductView Lite functionality and its differences with the thick client, thumbnails, and Pro/ENGINEER integration. TC members previewed the annotation feature in Pro/ENGINEER for Drawingless Models, along with details of version 7.0 functionality. After committee members discussed the idea of publishing a group newsletter as a way to share information, Mike Kotha agreed to put one together from members’ contributions. Windchill Infrastructure shared contributions and suggestions from companies in North America, Europe, and Japan. PTC presented plans and goals for the next two versions of the Windchill solutions, and committee members compiled and prioritized topics for white papers and feedback to PTC. The primary areas of concern in the next few months will be system management and performance. Committee members will be working with PTC to identify performance metrics, functional requirements, and common use cases to be considered for future Windchill versions. Windchill Solutions kicked off with updates on the status of the European and Japanese Windchill TCs. The group then held discussions covering PTC’s new usability model as well as reporting capabilities. The TC will be working on these topics with a focus on next-generation Windchill functionality. In addition, ●

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The PDMLink work group continued discussion of Product Structure Management focusing on view management, annotation set, configuration management and the needs of the federal, aerospace and defense industries for parts list management. The PartsLink/Classification work group reviewed functionality for the next release, and several users discussed their current needs and issues with the system. The ProjectLink work group spent time covering ProjectLink-specific reporting, along with user issues such as project management and secure server options.

The Winchill Solutions TC members expressed the desire for more communication with the Windchill Infrastructure TC, as well as with their European and Japanese counterparts. Several webcasts are planned before the June TC meetings to enable further discussion on the above topics. Meanwhile, in Europe… The European Simulation Technical Committee also convened in January, with 13 members in attendance. The objective for 2004 is to grow the European Simulation TC community. The plan includes starting a ProjectLink knowledge database on simulation techniques and to hold a tips and tricks session at each meeting. Committee members are also working with PTC to increase the committee’s communication with PTC product managers. PTC/USER World Event Once again the PTC/USER World Event will feature a “Meet Your Technical

Committee Breakfast.” This is where you can learn more about the specific activities of each group. Note that the following TCs are actively seeking new members: ● ● ● ● ●

Customization Data Exchange and Archiving Routed Systems (esp. ECAD and Pro/PIPING) Sheet Metal (esp. for Wildfire 3.0 project) Windchill Intrastructure

Your participation in a PTC/USER Technical Committee is the most direct way you can engage in the PTC product enhancement process. For more information, visit www.ptcuser.org/tc . Evan Caille can be reached by e-mail at [email protected].

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PTC/USER members will embark on a journey of discovery at the 2004 World Event this June in Nashville. “Discover,” this year’s theme, celebrates the spirit of learning and aspirations for achievement. Product development is a journey entailing risks and unknowns. To successfully meet the challenges, you need to tap into the knowledge from experts who have been in the trenches and understand the issues you face. The PTC/USER World Event is the only place you can meet hundreds of your peers in every industry from around the world. Here are a few of the highlights for 2004:

“Managing and Driving Models Using Skeleton Assemblies, BMX and MDX”

“I have been attending the conference for the last five years and it has been very beneficial for my organization. I always bring back information that I share with the Pro/ E users, especially in core modeling, large assembly management and routed systems.”

“The Dos and Don’ts of Migrating from Pro/ INTRALINK to PDMLink”

--Lorenzo C. Asia, Sandia National Laboratories

Over sixty technical presentations created for 2004, with more than half of these by experts from the PTC/USER community. Take advantage of the expertise and experience of top users. Sample topics include: “Large Assembly Management 101” “User-Defined Features: From Mystery to Magic”

Check out the complete list of expert presentations, PTC Product Update Briefings, and Best Practice Sessions. Tips & Tricks. You asked for it, you got it! The Tips and Tricks Contest returns bigger and better than before. It’s your chance to gain recognition from your peers and win valuable prizes. New Hands-On Workshops. PTC is offering two new sessions where you can try Pro/ENGINEER® Wildfire™ and receive a free 60-day trial edition. Novices can opt for an Introduction to 3D CAD while power users can step up to the next level with an Introduction to Pro/ENGINEER Wildfire 2.0. State-of-the-art networking. PTC/USER is introducing some cutting-edge technology to enhance your experience. Developed by nTAG based upon

research conducted at the MIT Media Lab, these “smart badges” will improve your ability to meet other attendees sharing your interests. Huge 22,000 square foot exhibit hall. One of the perennial favorites among members, the Exhibit Hall is the place to find the latest innovations from PTC and our Industry Partners. See demonstrations of software and other products by knowledgeable engineers. In addition, the Exhibit Hall will feature the Cyber Café, offering free e-mail and web access so you can easily keep in touch with your office and family. At the PTC Pavilion, you can schedule individual consultations with PTC Technical Support, Licensing, and Global Services staff. The conference will be held June 13-16 at the spectacular Gaylord Opryland Resort & Convention Center in Nashville, Tennessee. This incredible facility boasts some of the most comprehensive meeting facilities in the nation served up with a generous helping of Southern hospitality. Under the Opryland’s signature glass dome, you will discover nine acres of lavish gardens and cascading waterfalls and every amenity you can imagine. Jack Daniel’s Saloon and the Old Hickory Steakhouse are among fifteen top-notch dining options and five lively lounges where you can unwind with fellow attendees after your sessions. Relax at one of three pools or work off stress at the Gaylord Opryland’s fitness center.

PTC/USER guests will receive at no additional charge premium view accommodations with balconies overlooking the indoor gardens (availability on a first-come, first-served basis) along with complimentary transportation between the hotel and Nashville International Airport. Discover why hundreds of companies send their staffs to PTC/USER year after year. See the PTC/USER website for complete details about the event. You also

can download a color brochure of the event information (PDF format). We hope to see you in June! Rick Snider is Executive Director of PTC/USER and is also the webmaster for the ptcuser.org site. He can be reached at [email protected].

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I wanted to create a standard note that would list the material, hardness and finish of my part. To do so, I had two requirements. The first was to link the note to my part file in case my drawing was lost or corrupted. That way, the information would still reside in my part file. The other requirement was that if one of the three conditions did not apply, the note would be automatically renumbered and the extra note line removed. Here’s how to create a standard drawing note that is linked to parameters in your part file. 1. Modify the start part to contain six text string parameters. In this example, they are called NOTE1, NOTE2, NOTE3, MATERIAL, HARDNESS and FINISH (Fig. 1).

Note that it is important to add the parameters to your part before adding the relations. If you don’t, you will get errors when you try to save your relations. 2. Add the following relations to the start part.

NOTE1= "1. MATERIAL: " + material IF hardness == "NONE" IF finish == "NONE" NOTE2 = " " ELSE NOTE2 = "2. FINISH: " + finish ENDIF NOTE3= " " ELSE NOTE2 = "2. HARDNESS: " + hardness IF finish == "NONE" NOTE3 = " " ELSE NOTE3 = "3. FINISH: " + finish ENDIF ENDIF 3. Create and save a copy of your standard drawing note so you can reuse it in all your drawings. Here is the body of my standard note. {0:NOTES:} {1: }{2:&NOTE1} {3: }{4:&NOTE2} {5: }{6:&NOTE3} 4. When placed on the drawing, this is what your standard note will look like. NOTES: 1. MATERIAL: A-2 TOOL STEEL 2. HARDNESS: Rc: 58-62 3. FINISH: BLACK OXIDE Keep in mind that the part you are working with must be the “active” part in the drawing when you add the note. Kenneth S. Johnson is an associate industrial engineer at ITT Industries, Engineered Process Solutions Group. He can be reached by email at [email protected].

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Pro/ENGINEER allows you to attach any number of materials to the part database, but you can only assign one material to the part at any given time. What if the requirement is to have different materials for the instances of a part with family table? This technique lets you access parameters from one of the many material files defined in the generic model to drive the instances. 1. Construct a simple model with one circular protrusion.

2. Select Modify, Dimcosmetics, Symbol to change the symbol text of the dimensions to DIA and THICKNESS. 3. Select Part, Setup, Parameters to create the following set of parameters: Name

Type

Value

MATERIAL

STRING

STEEL

DENSITY

REAL NUMBER

0.0

VOLUME

REAL NUMBER

0.0

MASS

REAL NUMBER

0.0

UNIT_MATL_COST

REAL NUMBER

25

MATL_COST

REAL NUMBER

0.0

Note: If you set the config option new_parameter_ui to “yes”, you can work with the parameter editor. 4. To define the materials for your model, choose Part, Setup, Material, Define. Enter the names of the material files and the values for the mass densities as shown in the table below. (Since our objective is to capture the value of the density from the material file, I’ve only assigned values for the MASS_DENSITY parameters of the corresponding material files.) Name of the Material

MASS_DENSITY

STEEL

.00000784

ALUMINUM

.000002643

COPPER

.0000089

BRASS

.000008553

TITANIUM

.0000045

RUBBER

.000001506

HDPE

.000000955

5. Assign the materials defined in step 4. 6. Create the family table by adding both the diameter and thickness dimensions, plus the parameters created in step 3.

7. Select Insert, Datum, Analysis to create an analysis feature to compute the volume of the model.

8. From the Analysis definition dialog, enter MASS_PROP in the “Name” field and press Enter. 9. Click on the Model Analysis button and press Next.

10. Press the Compute button from the “Model Analysis” dialog, and then press Close.

11. As a final step in the creation of the analysis feature, enter VOL in the “Param name” field and then click on the green check mark.

The analysis feature you’ve just created calculates the mass properties each time the model is regenerated. 12. Now the stage is set for the magic…Select Part, Relations, Edit Rel and enter the relations exactly as shown below. /* IF VALUE FOR THE PARAMETER "MATERIAL" IS ENTERED WRONGLY, DEFAULTS TO STEEL IF(MATERIAL == "STEEL" | MATERIAL == "COPPER" | MATERIAL == "ALLUMINIUM" | MATERIAL == "HDPE" |\ MATERIAL == "BRASS" | MATERIAL == "RUBBER" | MATERIAL == "TITANIUM") MATERIAL=MATERIAL ELSE MATERIAL="STEEL" ENDIF /*Captures the density from the material file DENSITY=material_param("MASS_DENSITY",MATERIAL) /* Captures volume of the model from the analysis feature VOLUME=CEIL(VOL:FID_MASS_PROP,2)

/* Calculates mass of the model MASS=CEIL((DENSITY*VOLUME),2) /* Assigns the correct unit material cost always per the material if (material=="STEEL") UNIT_MATL_COST=25 endif if (material=="HDPE") UNIT_MATL_COST=125 endif if (material=="BRASS") UNIT_MATL_COST=175 endif if (material=="TITANIUM") UNIT_MATL_COST=500 endif if (material=="RUBBER") UNIT_MATL_COST=125 endif if (material=="COPPER") UNIT_MATL_COST=150 endif if (material=="ALLUMINIUM") UNIT_MATL_COST=75 endif /* Caluculates material cost of the model MATL_COST=CEIL((UNIT_MATL_COST*MASS),2) 13. Open the family table and verify the instances. 14. Now try changing the material parameter from the family table. The corresponding density is picked up automatically from the material file. The values for mass, unit material cost, material cost, etc. update as well. Some Final Tips ●

●

When you enter the value for the material parameter in the family table, be sure to fill in the exact name (without extension). Each time you modify the family table, remember to verify the instances.

Dwaraka Nadha Reddy.M is a design engineer (consultant) at Motor Control Centers, GE-IBC in Hyderabad, India. He can be reached by email at [email protected].