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Mold Design Tools Overview

This overview lists typical mold design tasks and the SOLIDWORKS functions that provide solutions to help you complete those tasks.

Task categories:

Procedural	Procedural tools create the mold and tools that enable you to display the model along different stages.
Diagnostic	Diagnostic tools show problem areas on the model. As you create the mold, you can examine the model for potential problems that might prevent the core and cavity from separating.
Corrective	Corrective tools repair the flaws, such as surface gaps, discovered by the diagnostic tools
Administrative	Administrative tools manage the models, facilitating the flow of information between designers, engineers, manufacturers, and managers.

Procedural

Tasks

Solutions

When you are not using models built with SOLIDWORKS, import parts into SOLIDWORKS.

Use the Import/Export tools to import models into SOLIDWORKS from another application.

The model geometry in imported parts can include imperfections such as gaps between surfaces. The SOLIDWORKS application includes an import diagnostic tool to address these issues.

Determine if a model (imported or built in SOLIDWORKS) includes faces without draft.

Use the Draft Analysis

tool to examine the faces to ensure sufficient draft. Additional functionality includes:

Face classification	Display color-coded count of faces with positive draft, faces with negative draft, faces with insufficient draft, and straddle faces.
Gradual transition	Display the draft angle as it changes within each face.

Check for undercut areas.

Use the Undercut Analysis

tool to locate trapped areas in a model that prevent ejection from the mold.

These areas require a mechanism called a “side core” to produce the undercut relief. Side cores eject from the mold as it is opened.

Scale the model.

Resize the model's geometry with the Scale Scale

tool to account for the shrink factor when plastic cools. For odd shaped parts and glass filled plastics, you can specify nonlinear values.

Select the parting lines from which you create the parting surface.

Generate parting lines with the Parting Lines

tool that selects a preferred parting line around the model.

Create shut-off surfaces to prevent leakage between core and cavity.

Detect possible sets of holes and automatically shut them off with the Shut-off Surfaces

tool. The tool creates surfaces to fill the open holes using no fill, tangent fill, contact fill, or a combination of the three. The no fill option is used to exclude one or more through holes so you can manually create their shut-off surfaces. You can then create the core and cavity.

Create the parting surface, from which you can create the tooling split.

With certain models, use the ruled surface tool to create interlock surfaces along the edges of the parting surface.

Use the Parting Surface

tool to extrude surfaces from the parting lines generated earlier. These surfaces are used to separate the mold cavity geometry from the mold core geometry.

Add interlock surfaces to the model.

Apply these solutions for interlock surfaces:

Simpler models. Use the automated option that is part of the Tooling Split tool.
More complex models. Use the Ruled Surface tool to create the interlock surfaces.

Perform tooling split to separate core and cavity.

Create the core and cavity automatically with the Tooling Split

tool. The Tooling Split tool uses the parting line, shut off surfaces, and parting surfaces information to create the core and cavity, and allows you to specify the block sizes.

Create side cores, lifters, and trimmed ejector pins.

Use Core

to extract geometry from the tooling solid to create a core feature. You can also create lifters and trimmed ejector pins.

Display the core and cavity transparently, enabling you to view the model inside.

Assign different colors to each entity with the Edit Appearance

tool. The Edit Appearance tool also manipulates optical properties such as transparency.

Display the core and cavity separated.

Separate the core and cavity at a specified distance with the Move/Copy Bodies

tool.

Diagnostic

Tasks	Solutions
Verify the integrity of imported parts. With imported or SOLIDWORKS parts, you can use the Scale tool as a validity check.	Use Import Diagnostics (Tools toolbar) to diagnose and repair gaps and flawed faces on imported features. Use Heal Edges to repair short edges on imported features. Use the Check tool to examine the imported model. For models with more severe imperfections, the SOLIDWORKS application includes other tools such as Filled Surface and Replace Face .
Ensure tangency between pairs of faces.	Calculate the angle and measure the boundary between faces with the Deviation Analysis tool. The analysis is based on the number of sample points that you select along the edges.
Find areas of model geometry that prevent ejection from the mold.	Identify problem areas in the model geometry with the Undercut Analysis tool.
Determine why knit faces operation fails. Some complex models may require you to use modeling techniques such as fill surface in conjunction with replace face to correct surface areas. When you knit these surfaces, they may fail because of gaps or interference between the surfaces.	Use the Check tool to examine the model. You can also use the Check tool with solids to examine imported data.

Corrective

Tasks

Solutions

With imported models, you can use the Diagnosis tool to repair gaps and flawed faces. If the gaps are too severe for the Diagnosis tool, apply the solutions described in this section.

Correct flaws to imported models (for example, model with surface gaps).

Correct flaws in the model with these SOLIDWORKS tools:

Filled Surface

Constructs a surface patch with any number of sides, within a boundary defined by existing model edges, sketches, or curves.

Replace Face

Replace faces in a surface or solid body with new surface bodies.

Move Face

Offset, translate, and rotate faces and features directly on solid or surface models.

Delete Face

Options include:

Delete and Patch	Deletes a face from a surface body or solid body and automatically patches and trims the body.
Delete and Fill	Deletes faces and generates a single face to close any gap.

Swept Surface

(See below.)

Lofted Surface

(See below.)

Knit faces, most likely used in conjunction with other modeling operations to attach new surfaces to the existing part.

Use the Knit Surface

tool to combine two or more faces and surfaces into one.

Add draft to models that include faces with insufficient draft.

Apply draft with the Draft

tool.

With some models (either imported or built with SOLIDWORKS), you can use the Draft tool to add draft. With other models, you need to move or create surfaces to change the draft angle.

Apply draft by using Move Face

to rotate a face to a specified draft angle.

Apply draft with SOLIDWORKS surfacing techniques. You can correct draft with the SOLIDWORKS surfacing techniques listed by building new surfaces with the correct draft angle. Then you can use Replace Face to incorporate these surface into the part.

Surface modeling techniques include:

Ruled Surface	Create surfaces that are either perpendicular or tapered away from selected edges.
Swept Surface	Start with an edge and create a surface sweep, using a guide curve when necessary.
Lofted Surface	Use existing profiles and create a surface loft, using a guide curve when necessary.
Filled Surface	Constructs a surface patch with any number of sides, within a boundary defined by existing model edges, sketches, or curves.

Split straddle faces

Do one of the following:

Use the Split Line tool to create silhouette curves along cylindrical faces. This splits the part and enables a parting line to generate.
Use the Split faces option in the Parting Lines tool.

Administrative

Tasks	Solutions
Track the evolution of a design or compare different designs.	Publish a eDrawings file, then send it to others who can use the free eDrawings Viewer to view the file. Add model-related information in the comments field. To learn more about eDrawings, click Help > Tutorials > All SOLIDWORKS Tutorials, and complete the eDrawings tutorial.
Manage product data and control revisions.	Use the SOLIDWORKS PDM add-in, a product data management tool. Click Tools > Add-Ins, and select SOLIDWORKS PDM to activate this add-in.
Replace an imported feature to incorporate a design change from the customer or supplier of the part.	Use Edit Feature to replace an imported feature with geometry from a new file. You can edit only features created from an ACIS, Autodesk Inventor, IGES, Parasolid, Pro/ENGINEER, Solid Edge, STEP, VDAFS, or VRML file.