­­SOLIDWORKS Tutorial: Master Modeling Techniques

Article by Jackie Yip on Aug 01, 2022

In SOLIDWORKS, propagating changes from one file is a smart strategy to control design flow. But the reality is that picking the source for where these changes occur can be a bit tricky. In this blog, we’ll demonstrate a workflow that fine-tunes this process when it comes to updating multiple parts inside an assembly.

­­SOLIDWORKS Tutorial: Master Modeling Techniques

This workflow is referred to as master modeling, where a single target, such as a sketch, can be modified to control multiple parts at the same time. The advantage of having this source is to speed up the design changes where a layout can be constructed to be the foundation for quick editing.

Creating the sketch & master part file

In this example, we’ll create different shapes that fit through a block. The sketch for the centerpiece contains the rectangular outline along with the shape profiles inside. In the part, we can reference this single sketch to allow it to be reused in multiple part files.

Creating a Sketch and Master Part File in SOLIDWORKS

In the same part file, we’ll extrude the inner contour to construct the rectangular plate with the shapes cut out. Once finished, the part will be saved out and will also serve as the master control file.

SOLIDWORKS Master Model Techniques

Reusing the master part file

In order the create the shapes as separate pieces, we’ll need to have a way to link it to the master source sketch. To do so, start a new part using the Insert Part command

Using SOLIDWORKS Insert Part Command on Master Model

The options to check the Absorbed sketches or Unabsorbed sketches will bring all sketches into the new part in their original form. Once completed, we’ll use each shape contour to extrude it to a new boss extrude and then save it as a new part.

Show Sketch SOLIDWORKS Master Model

Repeat this process for every shape. Once the parts are created, we will insert them into a new assembly.

SOLIDWORKS Assembly Master Model

Placing files into a new assembly

The trick to avoid using mates is to insert each component at its exact location where they were created by placing each component at the same origin. From the previous step, the Insert Part command allows each shape to remain in the same position where the master source sketch was used.

Placing Files into a New SOLIDWORKS Assembly

Editing the master part file

Once the parts are inserted inside the SOLIDWORKS assembly, feel free to open and edit the original master model and, from changing any element on the sketch, the parts will automatically update as well as thge assembly.

Editing Master SOLIDWORKS Part File

As desmonstrated above, any changes in the master part file will reflect the changes to the the existing parts and the assembly updates with relative ease.

GoEngineer YouTube Video SOLIDWORKS - Master Model Technique Want to learn more? Check out our YouTube video for a tutorial using SOLIDWORKS master model techniques. 

More SOLIDWORKS Assembly Tutorials

How to Save a SOLIDWORKS Assembly as an STL File

Create a SOLIDWORKS Assembly from a Multibody Part

Propagating Assembly Features to Parts

Understanding Hierarchy of SOLIDWORKS Appearances

SOLIDWORKS Tutorial: Creating and Dissolving Subassemblies

VIEW ALL SOLIDWORKS TUTORIALS

About Jackie Yip

Jackie Yip is a Technical Support Engineer at GoEngineer. When Jackie isn’t assisting customers or teaching a SOLIDWORKS Essentials class, he enjoys road biking and keeping up on the latest tech trends.

View all posts by Jackie Yip