Tool and Die Design Tools Overview

This overview lists typical tool and die design tasks and the SOLIDWORKS solutions that help you complete them.

Task categories

Importing Models from Other Applications

Tasks Solutions
In the SOLIDWORKS software, open a model created in a different CAD platform. Use the Import/Export tools to import models into the SOLIDWORKS software from another application.
Check an imported model for problems (gaps, bad faces), and fix any problems found. Use Import Diagnostics (Tools toolbar) to diagnose and repair gaps and flawed faces on imported features.

Use Check (Tools toolbar) to examine the imported model.

Use Heal Edges (Features toolbar) to repair short edges on imported features.

If flaws are too severe to correct with the Diagnosis tool, apply these solutions:

  • Move Face (Features toolbar). Offsets, translates, and rotates faces and features directly on solid or surface models.
  • Delete Face (Surfaces toolbar). Options include:
    Delete Deletes a face from a surface body, or deletes one or more faces from a solid body to create surfaces.
    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.
  • Filled Surface (Surfaces toolbar). Constructs a surface patch with any number of sides, within a boundary defined by existing model edges, sketches, or curves.
  • Replace Face (Surfaces toolbar). Replaces faces in a surface or solid body with new surface bodies.
  • Other surface tools. See Surfaces Toolbar.
Import geometry from other applications as reference geometry into SOLIDWORKS part documents. Imported Geometry imports surfaces, solids, sketches, curves, and graphics models as reference geometry into part documents.
Replace one imported body with another to support design changes. Edit an imported body or feature in a part by right-clicking it and selecting Edit Feature.
Change features in an imported model into features that the SOLIDWORKS software recognizes. Use FeatureWorks. Click Insert > FeatureWorks and then click Recognize Features or Options.

To learn more about FeatureWorks, click > Tutorials > All SOLIDWORKS Tutorials and complete the FeatureWorks tutorial.

Convert a 2D imported drawing into a 3D model. Use 2D to 3D conversion tools.
Insert a DXF or DWG file as a sketch in a SOLIDWORKS part document. Insert > DXF/DWG inserts a DXF or DWG file directly into the current SOLIDWORKS part document. You can then use the inserted sketch to modify the part.

Maintaining Relationships Between Parts

Tasks Solutions
Create a tooling part that uses the geometry of the customer part to define features. Use one of the following techniques:
  • Create a multibody part by using Insert Part (for parts created in SOLIDWORKS) or Imported Geometry (for parts created in other applications) to insert the customer part into the tooling part document. Then use Combine with Add, Subtract, or Common to manipulate the part.
  • To create tooling for molded parts, use mold design tools.

To learn more about mold design tools, click > Tutorials > All SOLIDWORKS Tutorials and complete the Mold Design tutorial.
Make the geometry of the customer part available in an assembly. In an assembly document, insert the customer part as a component. Then create parts in the context of the assembly, using the geometry of the customer part to define the tooling part within the assembly.
Define the overall shape of the tooling, and then split it into separate pieces. Use Split to split a part into multiple bodies. You can save each body in a separate part document, and then form an assembly from the new parts.

To learn more about maintaining associativity while splitting parts, click > Tutorials > All SOLIDWORKS Tutorials and complete the Molded Product Design - Advanced tutorial.

Use a layout to define where each component belongs in an assembly. In an assembly document, create an assembly layout sketch to verify that you positioned the components properly.
Use existing geometry in a part or assembly to define curves in a sketch for new geometry. Convert Entities projects an existing edge, loop, face, curve, external sketch contour, set of edges, or set of curves onto the sketch plane. Relations are created automatically that cause the new curve to update if the original entity changes.

Working with Sketches and Parts

Tasks Solutions
Create parts. Create sketches to add shapes (called features) to create parts.
Design sheet metal parts. Use Sheet Metal tools to create sheet metal parts. You can also use Convert to Sheet Metal.

To learn more about sheet metal, click > Tutorials > All SOLIDWORKS Tutorials and complete the Sheet Metal tutorial.

Create multiple versions of parts or assemblies within a single document. Create different configurations of a part in a single document. You can create configurations using any of the following methods:

To learn more about creating configurations using design tables, click > Tutorials > All SOLIDWORKS Tutorials and complete the Design Tables tutorial.

Determine the volume and mass of parts. Mass Properties calculates a part's properties such as density, mass, volume, and so on.
Sketch spline curves to use in creating a solid or surface. Use 2D splines and 3D splines. When defining splines, you can use:
  • Curvature Combs to visualize the slope and curvature of sketch elements.
  • Inflection Points to show where the concavity of a spline changes.
  • Minimum Radius to identify the curve with the smallest radius and display its radial measurement.
Create complex geometry. SOLIDWORKS tools that you can use to create complex geometry include:
  • Boundary Boss/Base (Features toolbar). Boundary creates solid boss/base and cut features similar to solid extrude, loft, revolve, and sweep features. Boundary produces very high quality, accurate features useful for creating complex shapes for the consumer product design, medical, aerospace, and mold markets.
  • Deform (Features toolbar). Alters the shape of complex surfaces or solid models, without concern for the sketches or feature constraints used to create the models.
  • Indent (Features toolbar). Creates an offset pocket or protrusion feature on a target body that exactly matches the contour of a selected tool body, using thickness and clearance values to create the feature.
  • Flex (Features toolbar). Deforms complex models in an intuitive manner by bending, twisting, tapering, and stretching.
  • Wrap (Features toolbar). Wraps a sketch onto a face.
  • Replace Face (Surfaces toolbar). Replaces faces in a surface or solid body with new surface bodies.
  • Intersection Curve (Sketch toolbar). Opens a sketch and creates a sketched curve at the intersection, such as between a plane and a surface, a surface and a part, two surfaces, and so on.
  • Composite Curve (Curves toolbar). Creates a curve by combining selected curves, sketch geometry, and model edges into a single curve.
Create solid geometry from a surface model. Use Thicken (Features toolbar) to thicken surfaces into solids or to create solids from enclosed volumes.

Working with Assemblies

Tasks Solutions
Drive a part or assembly design using a layout. In an assembly, create an assembly layout sketch to verify that your components are positioned properly.
Add parts to an assembly. Create a new assembly from an existing part or assembly using Make Assembly from Part/Assembly . Then use several methods to add components to the assembly.

You can also create a part in the context of an assembly so you can use the geometry of other assembly components while designing the part. The new part is saved within the assembly file as a virtual component. You can save the new part in a separate part file so you can modify it independently from the assembly.

To learn more about assemblies, click > Tutorials > All SOLIDWORKS Tutorials and complete the Lesson 2 - Assemblies tutorial.

Replace one component with another. Use Replace Components to replace components and update the assembly.
Manipulate component location, orientation, and display states. Use Move Component and Rotate Component to move assembly components.

Use Display States to specify a separate display mode (Wireframe, Hidden Lines Removed, etc.) for each component in an assembly.

Control assembly movement and define the design intent.

For example, you can constrain a shaft to remain concentric to the cylinder in which it moves.

Use mate tools to add mate relations that control the movement of parts:

Standard mates define standard mate relations between components, such as concentric, parallel, perpendicular, and so on.

Gear mates control the rotation of one component with respect to another component.

Lock mates maintain the position and orientation between two components.

Rack and pinion mates allow linear translation of one component (the rack) to cause circular rotation in another component (the pinion), and vice versa.

Limit mates limit component movement to a specified range.

Width mates center a tab within the width of a groove.

SmartMates automatically add mates when you drop components into place.

Path mates constrain a selected point on a component to a path.

Universal joint mates drive the rotation of the output shaft of a universal joint by the rotation of the input shaft about its axis.

Hinge mates limit the movement between components to one rotational degree of freedom.

To learn more about mates, click > Tutorials > All SOLIDWORKS Tutorials and complete the Assembly Mates tutorial.

Create holes and add fasteners. Create holes for fasteners with Hole Wizard , then use Smart Fasteners to automatically add standard fasteners into the holes.

You can access a customizable library of standard parts using the SOLIDWORKS Toolbox Library add-in. Select a standard and the type of part that you want to insert, then drop the component into the assembly. For details, see Toolbox Help.

Click Tools > Add-Ins, and select SOLIDWORKS Toolbox Library to activate this add-in.

To learn more about SOLIDWORKS Toolbox, click > Tutorials > All SOLIDWORKS Tutorials and complete the Toolbox tutorial.

Create Smart Components that require the addition of associated components and features such as bolts and mounting holes. When you insert the Smart Component into an assembly, you can choose whether or not to insert the associated components and features.

To learn more about Smart Components, click > Tutorials > All SOLIDWORKS Tutorials and complete the Smart Components tutorial.

Build efficient, modular assemblies using subassemblies. See Working with Subassemblies for tips and links to related topics.
Troubleshoot problems that you have when moving assembly components, such as components that collide. Use Interference detection to check a file for components that interfere with each other. A list gives you the names of the components that interfere and the interference volume. The area of interference highlights in the graphics area.

Use the Collision Detection option when you move or rotate components to detect if multiple components collide.

Use Clearance Verification to verify the minimum distance between selected components.

If a problem with mates is causing problems with the assembly motion, use MateXpert to identify mate problems.

Maximize performance of large assemblies. Use lightweight components, which loads only a subset of a model's data in memory. The remaining model data loads on an as-needed basis. You can also open subassemblies as lightweight components.

Enable Large Assembly Settings to maximize system option settings for large assemblies.

Use SpeedPak to create a simplified representation of an assembly without losing references. SpeedPak can significantly improve performance when you work in large and complex assemblies and related drawings.

Simplify assemblies and vary the assembly design with component configurations.

Visualizing the Design

Tasks Solutions
Change the color of a part, or make it transparent. Edit Appearance (View toolbar) edits the appearance of selected entities or the entire model and changes optical properties such as transparency and shininess.
Make an assembly component transparent. Change Transparency (Assembly toolbar) makes an assembly component 75% transparent. You can also hide components temporarily to allow you to work with underlying components.
In multibodies, make the main body transparent when creating a Combine feature with the Subtract operation. Combining Bodies - Subtract. Under Main Body, select Make main body transparent to help you select Bodies to Subtract that may be difficult to select with an opaque main body.
Examine the curvature of a part or assembly. Curvature (View toolbar) displays a part or assembly with the surfaces rendered in different colors according to the local radius of curvature. You can also display numerical values for curvature and radius.
Check for small changes, wrinkles, or defects in a surface. Zebra Stripes (View toolbar) simulate the reflection of long stripes of light on a very shiny surface. They enable you to see small changes in a surface that might be hard to see with a standard display, and to visually determine what type of boundary (contact, tangent, or continuous curvature) exists between surfaces.
Create a section view of a part or assembly. Section View (View toolbar) displays a view of the model cut with a plane through the part or assembly. You can also create section views in drawings.
Create an exploded view of an assembly. Use Exploded View and drag parts in the graphics area to create an exploded view. You can also animate the exploding and collapsing of the assembly.
Check how a component interacts with other components when you move it in an assembly. To check how components interact in an assembly, use the Physical Dynamics option in Collision Detection. When you drag or rotate a component, it applies a force to any components it touches, so you see the realistic motion of assembly components.
Simulate the effect of motors, springs, and gravity on an assembly. To record and play back a simulation of movement, use Physical Simulation. You can add simulation elements, such as springs, motors, and gravity that move components.
Examine an assembly for interferences between components. Use Interference Detection to check a file for components that interfere with each other. The volume of interference highlights in the graphics area.

Use Clearance Verification to check the minimum distance between selected components.

Simulate motion of components. To display machine movement:
  • To check how components interact while you are creating an assembly, use the Physical Dynamics option in Collision Detection. When you drag or rotate a component, it applies a force to any components it touches, and you view the motion of assembly components.
  • To record and play back a simulation of movement, use SOLIDWORKS Motion.
You can
  • Create animations of models, such as a rotating or exploding model with the Assembly Motion level of Motion Studies.
  • Add more physics and realism to your animation with SOLIDWORKS Motion (available in SOLIDWORKS Premium). You can add Simulation Elements that move components, such as springs, motors, and gravity, to control and automate motion.

To learn more about motion studies, click > Tutorial > All SOLIDWORKS Tutorials and complete the Assembly Motion tutorial.

Working with Drawings

Tasks Solutions
Make drawings from a part or assembly. Use Make Drawing from Part/Assembly (Standard toolbar) to create a drawing.

To learn more about drawings, click > Tutorials > All SOLIDWORKS Tutorials and complete the Lesson 3 - Drawings and Advanced Drawings tutorials.

Insert a DXF or DWG file as a sketch in a SOLIDWORKS drawing document. Use Insert > DXF/DWG to insert a DXF or DWG file into a SOLIDWORKS drawing document.
Add views. The SOLIDWORKS software offers tools to create various drawing views:

Add detail views, section views, break views, and broken out sections to a drawing.

Use Alternate Position Views to superimpose one drawing view precisely on another. Use alternate position views to show the range of motion of an assembly.

Add dimensions and annotations from part and assembly documents. Model Items (Annotation toolbar) inserts dimensions and annotations from part and assembly documents into the drawing document.
Add annotations and balloons to views. Add Center Marks , Centerlines , Geometric Tolerance Symbols , Notes , Surface Finish Symbols , and other annotations.

In Options > Document Properties > Drafting Standard, specify defaults for center marks, centerlines, balloons, and dimensions to be inserted automatically on view creation.

Use AutoBalloon to automatically insert balloons in a drawing.
Add a bill of materials and other tables. Use Bill of Materials to add a bill of materials to a drawing.

You can create bills of materials in assembly files. After you save the assembly, you can insert the BOM into a referenced drawing.

You can also add hole tables, revision tables, and weldment cut lists.

File Management and Collaboration

Tasks Solutions
Manage product data and control revisions. Use one of the following product data management (PDM) add-ins:
  • SOLIDWORKS Enterprise PDM (separate installation and licensing)

    Click Tools > Add-Ins and select SOLIDWORKS Enterprise PDM to activate this add-in.

    To learn more about SOLIDWORKS Enterprise PDM, when you are logged in to a local file vault, click Help > SOLIDWORKS Enterprise PDM Help.

Share documents with other users when collaborating on the design of a model. The multi-user environment provides read and write access control, and tracking for two or more users working with the same files concurrently.
Get the newest version of a document. Reload the document to get the latest version.
Replace a component in an assembly document. Use Replace Components to replace components and update the assembly. See Replace PropertyManager.
Store documents in a common place. Use Save to save the assembly document and all referenced component documents.
Copy a document to use it in a new design. Use Save As to create a copy of a document with a different name that you can use in other designs.
Change the location where you store parts and subassemblies of an assembly. Edit part location to save parts or subassemblies of an assembly to a new location or file name.
Rename a SOLIDWORKS document (part, assembly, or drawing) without losing its references to other SOLIDWORKS documents. Use SOLIDWORKS File Utilities to perform tasks such as renaming, replacing, and moving SOLIDWORKS files. To access SOLIDWORKS File Utilities, in File Explorer, right-click a SOLIDWORKS file, click SOLIDWORKS, and click Rename, Replace, or Move.
Send part, assembly, and drawing documents to others for review. Publish a eDrawings file from SOLIDWORKS, then send it to others who can use the free eDrawings Viewer to view the file.

To learn more about eDrawings, click > Tutorials > All SOLIDWORKS Tutorials and complete the eDrawings tutorial.