Design Automation for Creo Tips n' Techniques

Check out this video on Design Automation for Creo Parametric from CadActive  & PTC Application Engineers. 

Presenters: Phil Cluckies (CadActive), Ben Bowman (CadActive), Lino Tozzi (Technical Specialist, Fellow), and Tom Quaglia  (Creo Segment Sales).

Overview

This 59-minute PTC Creo Tips & Techniques webcast shows how to improve model performance and assembly management in Creo Parametric, and how CadActive design automation tools build on native Creo features. It is aimed at Creo designers, engineers, and CAD administrators working with large assemblies, cabling, and piping. Phil Cluckies and Ben Bowman of CadActive, a PTC technology partner, present, with Lino Tozzi of PTC hosting; it includes live demos of model templates, published geometry, bulk designation editing in Excel, skeleton copy geometry, and automatic assembly.

Chapters

This video has chapters. Select them from the chapter menu in the video player.

• 0:00 to 2:39: Welcome, presenters, and agenda
• 2:39 to 7:17: About CadActive and the automation journey
• 7:17 to 10:48: Why model performance and assembly management matter
• 10:48 to 12:33: Quick wins: model tree errors, Reference Viewer, ModelCheck
• 12:33 to 15:51: Simplified reps: master, empty, and automatic
• 15:51 to 18:47: Config.pro options for large assemblies and drawings
• 18:47 to 22:01: CadActive web interface: configs, libraries, templates
• 22:01 to 27:15: Demo: applying a model template in Creo
• 27:15 to 29:31: Model vs component parameters and published geometry
• 29:31 to 33:31: Demo: publishing geometry on a library part
• 33:31 to 37:15: Demo: designations and the Excel designation map
• 37:15 to 41:30: Bulk parts, envelopes, shrink wraps, and skeletons
• 41:30 to 44:19: Assembly context vs external copy geometry
• 44:19 to 54:25: Demo: skeleton copy geometry and AutoAssemble
• 54:25 to 59:29: Product packaging, Q&A, and close

Key Takeaways

• Fixing red (failed) items in the Creo model tree gives an immediate improvement in how the model performs, and is one of the easiest performance wins.
• An empty simplified rep excludes everything in the model tree, so even a massive assembly opens instantly and users then choose what to bring into session.
• The open_simplified_rep_by_default config.pro option can either show a dialog listing the assembly's simplified reps on open, or open a named rep such as the empty rep automatically.
• The automatic rep, which replaced the older graphics and geometry reps around Creo 4, loads only the minimum needed to display the model and loads more on demand as you select items.
• Model parameters live on library parts and apply wherever the part is used (for example vendor or revision); component parameters, such as designations, apply only in the context of one assembly and must be unique.
• Assembly context copy geometry links both what is copied and where it is placed; external copy geometry links only the geometry, which makes it the lightest-weight option but means placement must be updated when the source moves.
• CadActive applications are built with Pro/TOOLKIT and Object TOOLKIT functions and, at the time of recording, were maintained for all Creo versions back to Creo 4.0.

What does CadActive offer Creo Parametric users?

CadActive is a PTC technology partner that builds automation software that runs inside Creo Parametric, combined with consulting on the more advanced Creo challenges such as routed systems (cabling and piping). Its focus areas are task automation (fewer clicks and less error), model performance, data connectivity without manual translation, and high-fidelity CAD models that support downstream uses such as work instructions. The presenters recommend a staged journey: first synchronise settings such as config.pro files, then standardise the data in models, and only then automate tasks such as drawing creation, batch non-graphical processing, or building models from Excel.

Watch: 2:39 to 7:17 (CadActive overview slides and the synchronise, standardise, automate approach)

Why do model performance and assembly management matter in Creo?

Poor assembly management in Creo costs time and value: waiting for models to open, models that cannot be spun, crashes that lose work, and collaboration problems when engineers design over each other's work or use out-of-date data. The bigger risk is that parts of the product, such as cable harnesses, never get designed in CAD at all, which pushes problems downstream into manufacturing. Overweight, unmeshable, or unopenable models also lose value for manufacturing, service, sales, marketing, and quality.

Watch: 7:17 to 10:48 (slides on the cost of poor model performance)

What are the quickest ways to improve Creo model performance?

The fastest wins in Creo Parametric are to remove the red errors from the model tree, then use the Reference Viewer to trace which references Creo has to resolve when a component is brought into memory. ModelCheck, which is native to Creo, can enforce design standards and filter out bad CAD such as orphaned datums, buried features, and circular references. The presenters note that ModelCheck is driven by back-end text files and can be difficult to configure, maintain, and deploy.

Watch: 10:48 to 12:33 (tip slide covering model tree errors, the Reference Viewer, and ModelCheck)

Which simplified reps should every large Creo assembly have?

Every large Creo assembly should have a master rep, an empty rep, and should make use of the automatic rep. Simplified reps are stored in the master assembly file and let you load only the portions you need, for example excluding all hardware. To modify a simplified rep, the master assembly file must be in session, so the presenters suggest managing standard simplified reps at team or division level.

• Master rep: Fully loads everything in the model tree. This is what opens by default.
• Empty rep: Explicitly excludes everything in the model tree, so even a very large assembly opens instantly and users decide what to bring into session.
• Automatic rep: Loads the minimum information needed to display the model, then dynamically loads more as you select components or edges. It replaced the separate graphics and geometry reps around Creo 4.

Watch: 12:33 to 15:51 (slide explaining master, empty, and automatic reps)

Which config.pro options help with large Creo assemblies?

Two config.pro options highlighted for large Creo assemblies are prehighlight_tree and open_simplified_rep_by_default. The prehighlight_tree option controls whether hovering over an item in the model tree highlights it in the graphics window, which costs computation in a very large assembly. The open_simplified_rep_by_default option can show a dialog listing all simplified reps when you open an assembly, so nothing loads until a rep is chosen, or it can open a specific rep such as the empty rep every time. This prevents users from accidentally opening a top-level assembly in master rep and waiting an hour or two for it to load.

The presenters also shared a link to a list of config.pro options for large assemblies and drawings, which they offered to circulate after the webcast.

Watch: 15:51 to 18:47 (slide on prehighlight_tree, open_simplified_rep_by_default, and drawing options)

How do CadActive model templates check and fix Creo models?

A CadActive model template defines what a good Creo model looks like (orientations, simplified reps, layers, sections, and required parameters), and the Apply Model Template command compares a model against it and adds what is missing. Templates are managed in the CadActive web interface, which also manages standard config.pro profiles (for example a cabling profile for harness designers) and spec-driven piping libraries, writing the files Creo's piping module needs. Simplified rep rules in templates are based on the same search function as Ctrl+F in Creo.

1. Open Apply Model Template: On the CadActive tab in Creo, select Apply Model Template. It looks up the templates in your organisation and remembers the template last used on the model through a stored parameter.
2. Review the status indicators: Show details lists orientations, simplified reps, layers, sections, and parameters. Green means correct, yellow means the item exists but does not match (for example a view saved in the wrong orientation), and red means it is missing.
3. Check parameter types: Parameters are labelled Company (template standard), PTC (Windchill parameters), CadActive, or Custom. Custom parameters are left untouched.
4. Apply: Select Apply Selected for chosen items or Apply Template for everything. In the demo, deleted and skewed views, three default sections, and missing simplified reps were restored in one step.

Watch: 18:47 to 27:15 (web interface tour, then a live repair of views, sections, and simplified reps)

What is the difference between model parameters and component parameters in Creo?

Model parameters live on the part in the library and travel with it into every assembly, for example vendor information or revision number. Component parameters are applied to a component only in the context of a specific assembly. Designations are the most common component parameter: they distinguish identical pieces of equipment (pump 1, pump 2, pump 3) and must be unique in the model. Published geometry is a related model feature that identifies critical interfaces, surfaces, or datums on a library part so later design steps can be automated.

Watch: 27:15 to 29:31 (definition slides for model parameters, component parameters, and published geometry)

How do I publish geometry on a Creo library part?

Publish geometry on the library part once, so the interfaces are available every time the part is placed; CadActive's Geometry Publisher speeds this up. In the demo, an electrical component has published mounting surfaces and a coordinate system at each connector location, which are later used to constrain parts and to create copy geometry in skeletons quickly. Publishing and designations are native Creo features; the CadActive tools make them faster to create and lower the knowledge barrier.

1. Select datums to publish: Geometry Publisher lists all planes, points, axes, and coordinate systems. Select individual items, or use the checkbox to publish all of one datum type.
2. Publish: The tool creates the published geometry features, groups them, and moves them to the footer of the model tree. All published features can also be removed with one click.
3. Create a surface group: Choose the new surface group option, Ctrl-select the surfaces (in the demo, the mounting surface), middle-click to confirm, and enter a name.

Watch: 29:31 to 33:31 (live demo of publishing coordinate systems and a mounting surface group)

How can I bulk edit designations in a Creo assembly with Excel?

CadActive's designation tool can export a designation map to a CSV file, which you edit in Excel and import back into the Creo assembly. The CSV lists the feature number, component path, and model name in model tree order, so you can copy, paste, drag-fill, and use formulas on designations in bulk. On import, status indicators flag conflicts: red marks the duplicated designation and yellow marks a subassembly containing one, so you can drill down and fix each until everything is green.

1. Create the designation map: Use Create Designation Map to write the assembly's designations to a CSV file.
2. Edit in Excel: Change designations in bulk with copy and paste, fill, or formulas, then save the file.
3. Import and resolve conflicts: Import the map, expand any yellow subassemblies, and edit red entries until all indicators are green.

Component parameters can be exported, edited in Excel, and re-imported the same way.

Watch: 33:31 to 37:15 (export to Excel, bulk editing, and resolving duplicate designations)

When should I use bulk parts, envelopes, shrink wraps, and skeletons in Creo?

Use bulk parts for items that only need to appear in the bill of materials, such as fasteners, paint, sealant, or glue; envelopes and shrink wraps to claim space for a component without loading its detail; and skeleton models when several engineers contribute to a large assembly. For example, you may only need to know where a battery or control box sits, not its internals. Envelopes and shrink wraps are powerful but can be harmful if used incorrectly. CadActive's best practice for larger models is to create skeleton models of the higher-level assemblies and populate them with copy geometry.

Watch: 37:15 to 41:30 (lightweight representation slides and the live answer on shrink wrap errors)

What is the difference between assembly context and external copy geometry in Creo?

Every copy geometry feature answers two questions, what is copied and where it is placed, and the difference lies in the where. Assembly context copy geometry is fully associative: both the geometry and its placement stay linked to the source model in the larger assembly. External copy geometry keeps the geometry linked but leaves placement to the user, so if the source component moves you must update it manually. External copy geometry gives the lightest-weight model possible.

Watch: 41:30 to 44:19 (explanation of the what and where of copy geometry types)

How do I build a skeleton with copy geometry and auto-assemble components in Creo?

In the demo, CadActive's copy geometry tool (Geometry Copier) creates external copy geometry in a skeleton for every published geometry feature in an assembly, and AutoAssemble then places components onto that geometry from a schematic file. Each component gets a component placement coordinate system in the skeleton, which locates its copy geometry and lets associativity be restored when the source moves.

1. Create the subassembly: Create a subassembly with a contained skeleton, and optionally a harness part for cabling.
2. Copy all published geometry: Select the equipment assembly and the target skeleton, then use copy all children at the top level. In the demo this created a little over 100 features in one click.
3. Tidy the tree: Use the option to fix copy geometry groups, which groups features by the component they reference.
4. Run AutoAssemble: Select an NWF file exported from a 2D schematic tool. Components come in with their designations, including connectors with backshells assembled onto them.
5. Update after a move: If a source component moves, right-click it in the skeleton, select Update Location, and regenerate. The connectors snap back into place.

The same approach applies beyond cabling, for example to configurable assemblies built from Excel.

Watch: 44:19 to 54:25 (live skeleton build, automatic assembly of over 100 components, and Update Location)

How are CadActive's Creo tools packaged?

CadActive packages its Creo tools to follow the synchronise, standardise, automate approach, with automation that includes drawing automation, building models from Excel, command-line and non-graphical bulk processing, and automatic assembly. Piping and cabling are a large part of its work but not the limit, and a reporting module can pull information from Creo on demand or automatically. Lino Tozzi of PTC summarises it as Creo toolkit automation that takes Creo to the next tier for very manual processes.

Watch: 54:25 to 56:22 (product packaging slide and PTC's summary)

Frequently Asked Questions

Q: Why can envelopes and shrink wraps cause errors in Creo if used incorrectly?

A: A shrink wrap is a collection of copy geometry features that can reference a whole assembly. If referenced geometry changes and a reference is lost, the error is hard to troubleshoot at that granular level, and the usual fix is to delete and recreate the shrink wrap. Lino Tozzi adds that they only simplify what already exists, so they will not create errors unless the source already has them; the real risk is extra work when they are used without a clear purpose. (answered at 40:18 and 56:48)

Q: Can published geometry be used for cabling and harnesses in Creo?

A: Yes. The skeleton and AutoAssemble demo used a cabling assembly with a harness part, and the presenters stress that copy geometry should be used in all large assembly management, not just cabling. (answered at 56:32)

Q: Do I need the master assembly in session to edit a simplified rep?

A: Yes. To modify a simplified representation, the master assembly file must be in session, which is why standard simplified reps are best managed at team or division level. (12:53)

Q: Which Creo versions do CadActive tools support?

A: At the time of recording, CadActive said it maintained and built its application for all Creo versions back to Creo 4.0. (5:28)

Links & Resources

• CadActive (cadactive.com)
• Geometry Publisher: Publish Geometry (support.cadactive.com)
• Geometry Copier (support.cadactive.com)
• AutoAssemble (support.cadactive.com)
• About Simplified Representations (Creo help) (support.ptc.com)
• Creo Large Assembly Management Tips n' Techniques (community.ptc.com)