Repair Geometry by IDD

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Creo Tutorials Hub

Welcome to Our Creo Data Repair Hub!
Discover how the Import Data Doctor (IDD) transforms messy imported geometry into clean, usable Creo models. Whether you’re fixing STEP, IGES, or CATIA files, IDD gives you the tools to heal gaps, repair surfaces, and optimize foreign data for seamless design workflows.

Why Use the Import Data Doctor?

IDD is your go-to solution for:

  • Repairing broken geometry from non-Creo files (e.g., missing surfaces, misaligned edges).
  • Simplifying complex imports by removing redundant vertices or sliver faces.
  • Preparing models for 3D operations like extrusion, filleting, or shelling.

Learn with Tutorials

Below, you’ll find a list of tutorials to help you get started with Import Data Doctor (IDD)

Redefining Attributes & Surface Editing

Working with imported geometry in Creo Parametric? Whether you’re dealing with STEP, IGES, or other neutral CAD formats, understanding how to redefine imported attributes and modify surface entities is crucial for efficient modeling. This guide walks you through adjusting solid/surface conversion, joining adjacent surfaces, and selectively deleting unwanted entities—helping you clean up and optimize imported models.

Redefining Imported Attributes

When importing external geometry, Creo allows you to control how the data is interpreted. You can define whether the feature should be a solid or remain as surfaces, and whether adjacent surfaces should be automatically joined.

How to Redefine Imported Attributes

  1. Access the Feature Definition:
    • Right-click the imported feature in the Model Tree and select Edit Definition.
    • Alternatively, select the feature and go to Edit > Definition.
  2. Modify Feature Properties:
    • Click Edit > Feature Properties to open the Properties menu.
    • Choose from the following options:
      • Make Solid – Converts the imported data into a solid feature.
        • Note: Automatically enables Join Surfs if the geometry forms a closed volume.
      • Join Surfs – Merges surfaces that share boundaries where possible.
      • Join Layers – Combines layers of selected surfaces.
    Key Behavior:
    • If Make Solid is selected, Join Surfs is also enabled.
    • If the imported geometry is already a solid protrusion, both options remain selected.

Deleting Unwanted Entities from Imported Surfaces

Imported models often contain unnecessary reference geometry (curves, points, or datum planes) that clutter the workspace. Creo allows you to selectively remove these elements while preserving critical surfaces.

Step-by-Step Entity Deletion

  1. Enter Edit Mode:
    • Right-click the feature in the Model Tree and choose Edit Definition.
    • Or, go to Edit > Definition.
  2. Open the Delete Tool:
    • Click Edit > Delete to open the DELETE ENT menu.
  3. Choose Entity Types to Delete:
    By default, Creo selects:
    • Points
    • Datum Planes
    • Curves
    Toggle these options or enable Surfaces if needed.
  4. Select Items for Removal:
    • Click Select Item and use the SELECT menu to pick entities.
    • Click Done Sel to confirm or Rehighlight to review selections.
  5. Finalize Deletion:
    • Click Done in the DELETE ENT menu to apply changes.

Mastering Surface Joining & Repair in Creo Parametric

Working with imported surfaces in Creo? Whether you’re merging adjacent surfaces, excluding problematic areas, or fixing gaps, proper surface handling ensures clean, manufacturable models. This guide covers joining surfaces, excluding surfaces from quilts, and manual gap repair—essential skills for working with imported CAD data.

Joining Surfaces in an Imported Feature

  • Merges adjacent surfaces that share boundaries
  • Creates a single quilt from disjointed surfaces
  • Prepares watertight geometry for solid conversion

Step-by-Step Process

  1. Enter Edit Mode
    • Right-click the feature in the Model Tree > Edit Definition
    • Or use Edit > Definition
  2. Access Surface Joining
    • Click Edit > Feature Properties
    • By default, Make Solid and Join Surfs are selected
  3. Adjust Joining Options
    • To join surfaces without creating a solid:
      1. Clear Make Solid
      2. Re-select Join Surfs
    • Note: Clearing Join Surfs automatically deselects Make Solid
  4. Finalize & Repair
    • Click Done/Return to apply
    • Use Fix Bndries to repair imperfect joins

Excluding Surfaces from a Quilt

  • Isolates problematic surfaces
  • Prevents automatic joining of unwanted geometry
  • Allows selective surface editing

How to Exclude Surfaces

  1. Open Feature Properties
    • Right-click feature > Edit Definition > Edit > Feature Properties
  2. Enter Exclusion Mode
    • Click Exclude Surfs
    • Boundaries highlight in blue
  3. Modify Exclusion SetOptionActionAddIncludes surfaces in exclusionRemoveTakes surfaces out of exclusionRemove AllClears all exclusions
  4. Confirm Changes
    • Click Done → Excluded boundaries turn yellow

Limitations:

  • Some surfaces remain joined due to original import topology
  • Curvature discontinuities may prevent full exclusion

Closing Gaps & Fixing Tangency

  • Yellow edges indicate unresolved gaps
  • Surface tangency issues affect continuity
  • Warning: This process is non-reversible

Gap Repair Procedure

  1. Launch Manual Repair
    • Edit Definition > Geometry > Heal Geometry > Manual
  2. Choose Repair Type [ Zip Gaps ] – Closes physical gaps between edges [ Fix Tangency ] – Improves surface smoothness
  3. Select Edges
    • Use SEL CHAINS menu to pick edges
    • Click Done Sel after first selection
  4. Adjust Parameters
    • Set MAX VALUE for gap size/tolerances
    • System displays measurable angles/gaps
  5. Execute Repair
    • A red mesh previews changes
    • Unfixed edges stay blue
  6. Finalize
    • Accept → Confirms permanent changes
    • Reject → Abandons modifications

Pro Tip:
If gaps persist, increase tolerance values and repeat the process.

Best Practices for Imported Surface Repair

✅ Join Surfs First – Resolve major gaps before exclusions
✅ Use Small Increments – Gradually increase gap tolerance
✅ Backup First – Manual repairs can’t be undone
✅ Inspect Curvature – Check for underlying CAD issues

Master these techniques to transform messy imports into production-ready models! 🔧

Fixing Problem Boundaries

When working with imported geometry in Creo Parametric, surface boundaries often require special attention. This guide covers professional techniques for repairing problematic surfaces, including gap closure, tangency fixes, and boundary optimization. Mastering these tools will help you transform imperfect imports into production-ready models.

Surface Repair Workflow Overview

  1. Right-click the feature in the Model Tree
  2. Select Edit Definition
  3. Navigate to Geometry > Heal Geometry > Manual

The system provides five specialized repair options:

Repair OptionBest ForLimitations
Zip GapsClosing physical gaps between surfacesWorks best on small gaps
Fix TangencyImproving surface continuityOnly for angles <10°
FixQuiltBndrySimplifying complex boundariesRequires nearly tangential segments
Edit BndryManual boundary adjustmentAdvanced skill required
FixVerticesAligning misaligned verticesWorks on vertex sets

Detailed Repair Techniques

1. Zip Gaps – Closing Physical Gaps

When to use: When yellow edges indicate unjoined surfaces

Procedure:

  1. Select Zip Gaps from FIX OPTIONS
  2. Set maximum gap tolerance:
    • Use Default for initial attempt
    • Enter to specify exact values
  3. Select edges using:
    • Auto Select for automatic detection
    • Sel Chain for manual selection
  4. Review blue-highlighted edges
  5. Execute repair and verify results

Pro Tip: Start with the default value, then gradually increase if needed.

2. Fix Tangency – Improving Surface Flow

Prerequisites:

  • Complete gap closure first
  • Only works on angles <10°

Workflow:

  1. Choose Fix Tangency option
  2. Set MaxDihedral angle (default is recommended)
  3. Select problematic edges
  4. Review the red mesh preview
  5. Accept or Reject changes

Important: This action is non-reversible – consider saving first.

3. FixQuiltBndry – Boundary Optimization

Best for: Simplifying complex quilt edges

Step-by-Step:

  1. Select FixQuiltBndry
  2. System highlights qualifying segments (orange)
  3. Use Unsel Chain to exclude specific boundaries
  4. Click Done to execute
  5. Verify simplified boundaries

Visual Cues:

  • Orange: Candidate segments
  • Red: Excluded from repair

Configuration Options for Better Imports

Set these in your config.pro to automate some repairs:

fix_boundaries_on_import yes
intf3d_in_close_open_boundaries yes

Benefits:

  • Automatic boundary repair during import
  • Reduced manual cleanup
  • More consistent results

Selection Techniques (SEL CHAINS Menu)

Auto Select:

  • Fastest method
  • Based on MaxGapDist/MaxDihedral values
  • Can be interrupted with Stop sign

Manual Selection:

  • Single: Pick individual edges
  • Chain: Select connected edge sequences
  • Unsel Chain: Remove edges from selection

Best Practices for Boundary Repair

  1. Work progressively: Start with smallest tolerances
  2. Save frequently: Many repairs are non-parametric
  3. Combine methods: Use Zip Gaps before Fix Tangency
  4. Verify results: Check curvature continuity after repairs
  5. Document changes: Note tolerance values used

Troubleshooting Common Issues

Problem: Gaps won’t close
Solution:

  • Increase MaxGapDist incrementally
  • Check for underlying geometry issues

Problem: Tangency fixes fail
Solution:

  • Ensure gaps are closed first
  • Verify angle is <10°
  • Try smaller sections

Problem: Boundaries won’t simplify
Solution:

  • The segments may not be sufficiently tangential
  • Consider manual Edit Bndry instead

By mastering these advanced surface repair techniques, you’ll significantly improve your ability to work with challenging imported geometry in Creo Parametric. Remember that complex repairs may require multiple passes and combination of different methods.

Advanced Surface Repair Techniques

Boundary editing is a critical skill for working with complex imported surfaces in Creo Parametric. This comprehensive guide covers professional techniques for modifying, creating, and optimizing surface boundaries to achieve perfect geometry alignment and continuity.

Accessing Boundary Editing Tools

Navigation Path:

  1. Right-click feature in Model Tree → Edit Definition
  2. Navigate to Geometry > Heal Geometry > Manual
  3. Select Edit Bndry from FIX OPTIONS menu

Alternative access: Use Edit > Definition from the main menu

Boundary Selection Methods

Selecting Boundary Chains

  1. Select All – Chooses entire closed loops
  2. From-To – Selects between two specific vertices

Visual feedback: Selected edges highlight in red

Complete Boundary Editing Workflow

Step 1: Initial Setup

1. Select target surface 2. Choose boundary selection method 3. Confirm selection with Preview

Step 2: Boundary Modification Options

EDIT BNDRY Menu Functions:

CommandPurposeKey Considerations
CreateBuild new boundary edgesMaintains surface integrity
ModifyAdjust existing edgesPreserves geometric relationships
DeleteRemove unwanted edgesRequires replacement
CombineMerge multiple chainsEnsures continuity
Undo LastReverts last actionNon-destructive editing
PreviewVisualize changesCritical before finalizing
Geom CheckValidate surface qualityIdentifies problem areas
Set DomainControl mesh densityAffects modification precision

Step 3: Advanced Creation Techniques

CREATE Menu Options:

  • Project – Converts curves to surface edges
  • Make Isoline – Creates natural surface flow lines
    • Use Accept/Next to choose direction
    • Connect for point-to-point edges
    • Intersect for surface intersections

Step 4: Precision Modification Tools

MODIFY EDGS Menu Features:

  1. Straighten – Simplifies complex edges
  2. Merge Edges – Combines segmented edges
  3. Move Vertex – Repositions connection points
  4. SetTanCond – Controls edge continuity:
    • Start/End tangent management
    • Tangent/Normal/Free conditions
  5. Divide – Splits edges at specified points

Specialized Quilt Boundary Repair

FixQuiltBndry Procedure

  1. Identify problematic boundaries (yellow edges)
  2. System highlights candidate segments (orange)
  3. Use Unsel Chain to exclude specific edges
  4. Execute repair with Done

Visual Indicators:

  • Red: Excluded from repair
  • Orange: Candidate for optimization

Professional Tips & Best Practices

  1. Workflow Optimization
    • Always preview changes before finalizing
    • Use geometric checks frequently
    • Save incremental versions
  2. Advanced Techniques
    • Combine projection and isoline methods
    • Use tangency conditions for smooth transitions
    • Balance straightening with curvature requirements
  3. Troubleshooting
    • If edits fail, check for:
      • Open chain violations
      • Tangency conflicts
      • Surface continuity issues

Common Use Cases

  1. Aerospace Surfaces – Maintaining precise airflow characteristics
  2. Automotive Class-A – Ensuring perfect continuity
  3. Consumer Products – Creating manufacturable transitions
  4. Medical Devices – Meeting strict tolerance requirements

Conclusion

Mastering boundary editing in Creo Parametric enables you to:

  • Transform imperfect imports into production-ready models
  • Achieve perfect surface continuity
  • Solve complex geometric challenges
  • Reduce downstream manufacturing issues

Comprehensive Healing Process for Imported Geometry

1. Initial Boundary Assessment

  1. Access healing tools: Geometry > Heal Geometry > Manual > Edit Bndry
  2. Select boundary method:
    • Select All for complete loops
    • From-To for specific segments
  3. Run diagnostic: Geom Check to identify:
    • Overlapping geometry
    • Coincident surfaces
    • Boundary inconsistencies

2. Gap Closure Procedure

1. Navigate to: Geometry > Heal Geometry > Manual > Zip Gaps 2. Selection methods: [Auto Select] – Automatic chain selection • Adjust MaxGapDist incrementally [Sel Chain] – Manual edge selection 3. Execute Zip Gaps 4. Evaluate results via surface mesh preview

3. Geometry Validation Cycle

  1. Re-run Geom Check after each operation
  2. Address issues systematically:
    • Overlapping surfaces: Adjust boundary alignment
    • Self-intersections: Modify patch geometry
    • Invalid patches: Rebuild problematic areas

4. Vertex Correction

  1. Access: Geometry > Heal Geometry > Manual > FixVertices
  2. System automatically:
    • Aligns mispositioned vertices
    • Resolves connectivity issues
  3. Verify corrections with Geom Check

5. Tangency Optimization

  1. Select: Fix Tangency from manual repair menu
  2. Automatic selection of two-sided edges
  3. Manual override available for specific chains
  4. Evaluation criteria:
    • Surface continuity (G1)
    • Maximum 10° dihedral angle
  5. Accept/reject via ACCEPT FIX menu

6. Quilt Boundary Refinement

  1. Execute FixQuiltBndry to:
    • Simplify complex edges
    • Resolve multi-segment boundaries
  2. Visual indicators:
    • Orange: Candidate edges
    • Red: Excluded segments

7. Final Closure Operations

  1. For remaining holes:
    • Use Geometry > Collapse Geom
  2. Final validation:
    • Only quilt boundary checks should remain
    • All other geometry checks must be resolved

Professional Tips for Effective Healing

Workflow Optimization

  • Incremental approach: Make small changes between checks
  • Diagnostic hierarchy: Address overlaps before tangency
  • Parameter adjustment: Gradually increase MaxGapDist

Advanced Techniques

  1. For stubborn gaps:
    • Combine manual selection with auto-detect
    • Use 80% of known gap size as initial value
  2. For complex tangency:
    • Fix in small sections
    • Use Edit Bndry > SetTanCond for precise control

Quality Assurance

  1. Validation checklist:
    • No unexpected geometry checks
    • Smooth mesh display
    • Consistent edge highlighting
  2. Manufacturing considerations:
    • Verify draft angles
    • Check curvature continuity
    • Ensure watertight boundaries

Cleaning Up Imported Geometry in Creo Parametric

Pre-Import Preparation

Critical Configuration Settings

  • Absolute accuracy: Set based on:
    • Part size
    • Smallest edge to preserve
  • Recommended config options:configCopyfix_boundaries_on_import yes intf3d_in_close_open_boundaries yes

Post-Import Cleanup Strategies

Automatic vs. Manual Cleanup

MethodProsConsBest For
AutomaticFast results
Minimal user input		Changes parametrics
Less control		Initial cleanup
Simple geometry
ManualPrecise control
Preserves parametrics		Time-consuming
Requires expertise		Complex surfaces
Critical features

Step-by-Step Cleanup Workflow

1. Initial Assessment

  1. Run Geom Check diagnostics
  2. Identify:
    • Overlapping surfaces (red)
    • Coincident geometry (yellow)
    • Gaps > current accuracy

2. Automatic Cleanup Procedure

1. Right-click feature > Edit Definition 2. Geometry > Heal Geometry > Automatic 3. Surface selection: [Include] – Choose affected areas • Indiv Surfs – Single surfaces • Surf & Ngh – Surface + neighbors • All Surfs – Entire model [Exclude] – Protect critical geometry 4. Set constraints (optional) 5. Click Compute 6. Compare surfaces using Analysis

3. Manual Repair Techniques

For Problem Surfaces:

  1. Isolate problematic surfaces (place on blanked layer)
  2. Rebuild using:
    • Boundary Blend
    • Style surfaces
    • Conic patches

Common Fixes:

  • Overlapping surfaces: Edit Boundary > Create common edge
  • Singularities: Rebuild UV parameterization
  • Gaps: Zip Gaps with incremental MaxGapDist

4. Geometry Collapsing

  1. Create replacement parametric geometry
  2. Collapse Geometry to:
    • Add patches to imported feature
    • Remove distorted surfaces
  3. Verify:
    • No parent/child conflicts
    • Maintained surface continuity

Advanced Cleanup Techniques

Surface Analysis Tools

  • Mesh display: Check UV parameterization
    • Parallel lines indicate singularities
  • Deviation analysis: Compare original/repaired
  • Curvature combs: Verify edge continuity

Boundary Editing Pro Tips

  1. Vertex alignment > edge alignment
  2. Modify existing edges rather than create new
  3. Use Query Select for precise picking
  4. Domain meshes help visualize edits
  5. Save frequently – changes are non-parametric

Handling Mixed Data Types

For Combined Wireframe + Surfaces

  1. Process wireframe first
  2. Use as foundation for surface repair
  3. Apply standard cleanup techniques

For 2D/3D Combinations

  • Import as:
    • Part/Assembly for 3D data
    • Drawing for 2D data
  • Process separately then combine

Troubleshooting Guide

ProblemSolutionTool
Can’t fix boundaryExclude surface, recreateEdit Boundary
Internal yellow edgesMust fix before mergingJoin Surfs
SingularitiesRebuild parameterizationStyle
Persistent gapsIncrement MaxGapDistZip Gaps
Tangency failuresCheck angles <10°Fix Tangency

Best Practices Checklist

  • Set proper accuracy before import
  • Use automatic cleanup first pass
  • Address diagnostic errors in order
  • Save incremental versions
  • Verify with multiple analysis tools
  • Document tolerance values used

Mastering the Automatic Surface Cleanup in Creo Parametric

Dealing with imported geometry in Creo Parametric can be tricky, especially when surfaces are incomplete or disjointed. Fortunately, the Automatic Surface Cleanup tool provides a powerful set of options to clean up wireframes and surfaces. This guide walks you through the key functions available in the Automatic Surface Cleanup dialog box, how to apply constraints, use surface analysis, and collapse geometry to finalize your design.

Wireframe and Surface Modifications

When working with the Modify Wireframe menu, you have granular control over which geometry elements are included or excluded from the surface repair process.

  • Include > Edge chain: Select edge chains to include in the computation.
  • Exclude > Surface: Choose surfaces to exclude from the surface cleanup.
  • Exclude > Curve: Exclude specific curves from the computation.
  • Exclude > Vertex: Remove selected vertices from the process.
  • Suspend > Edge chain: Temporarily suspend edge chains to exclude them from cleanup.

Applying and Managing Constraints

In the Modify Constraints section, you can refine how surfaces interact by applying or removing different constraints:

  • Frozen / Frozen w/boundary: Lock surfaces with or without boundary edges.
  • Tangent: Add or remove tangency at selected edges.
  • Master: Define a master surface for controlling tangent behavior.
  • Split: Split or join surfaces along specific points.
  • Set Defaults: Revert all constraints to default settings.

Display Options – Visualizing Constraints and Geometry

You can visually review constraint settings using the Display Options:

  • Frozen: Shows all frozen surfaces with mesh and tags.
  • Master: Displays hashings on master edges.
  • Tags: Highlights all constraint tags in the model.
  • Fixed Srfs: Modified surfaces are shown in red for clarity.

Surface Computation & Confirmation

  • Compute: Run the cleanup operation and rebuild the surfaces.
  • Accept: Finalize the solution once surfaces are rebuilt.
  • Quit: Exit the automatic surface cleanup process.

Understanding Constraint Colors and Tags

Creo Parametric uses color-coded mesh and tags to visually identify constraints applied to surfaces:

Constraint TypeVisual Representation
FrozenDark cyan mesh with green “F” tag
Frozen w/BoundaryGray dense mesh with white “B” tag
MasterHashing on the master side of the edge
TangentCyan edge with cyan “T” tag
SplitCyan dotted line and “T” tag at tangent creation

These visual aids help users understand which constraints are active and where.

Surface Deviation Analysis

To analyze how much the cleaned-up geometry deviates from the original, use the Compare Surfaces tool (under Analysis > Surface Analysis > Compare Surfaces):

  • New Surface: Select changed, red-colored meshed surfaces.
  • New Geometry: Select all geometry and compare it to the original geometry.

Collapse Geometry – Finalizing Repaired Surfaces

When surface patches are deleted and holes appear, Collapse Geometry helps you repair them by merging imported geometry into new parametric features.

Workflow:

  1. Go to Geometry > Heal Geometry > Automatic or Manual to clean up the quilt.
  2. Create a parametric feature to fill any holes.
  3. Navigate to Geometry > Collapse Geometry.

SELECT FEAT Menu Options:

  • Select: Pick features for collapse.
  • Layer / Range: Access the Child menu for features with children.
  • Done: Apply the collapse and regenerate.
  • Quit: Cancel and return to the import menu.

Child Menu Options:

  • Show Ref: See references of highlighted feature.
  • Include / Include All: Collapse selected or all dependent features.
  • Suspend: Temporarily disable the highlighted feature.
  • Info: View feature information.
  • Quit: Return to the SELECT FEAT menu.

Tip: Avoid Merging Imported Features

Avoid manually merging Creo features created from imported geometry. These features will merge automatically when using the Collapse Geometry tool.

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