There are many ways to create your parts and assemblies in SOLIDWORKS. A common way is the so called “Bottom-Up” assembly method, where assemblies are created by adding existing parts in an assembly. Another approach is the “Top-Down” assembly method, where parts are created in the context of the assembly. In this tech blog, I want to focus on the master model technique, where parts are driven from a single part, which contains overall size, location and gross geometry for an entire assembly. Geometry detail is generally found in the individual part files. A big advantage is the time gain when you need to make model changes. In this case you just need to edit your master model and these changes are directly transferred to the derived parts.
The master model technique can be divided into two categories:
Let’s take a closer look at these two types.
This means that a solid master model (parent) is split into solid bodies, which are saved as individual part files (children). Figure 1 shows an example.
The following features are imported for this type of master model technique:
First you split the master model into multiple bodies with the Split feature, after that you save all the bodies to separate parts with the Save Bodies command. It is a good habit to create the details in the separate part files, because otherwise the master model will be too complex. Be aware that Save Bodies is inserted as a feature, so changes made after this feature will not be translated to the derived parts. If this is desired, then just drag and drop the Save Bodies feature to the end of the Feature Manager Design Tree.
In this case, the entire master model is brought into each child part and the design for each component proceeds from there. Figure 2 shows an example.
For this type of master model technique, it is imported to know the following feature:
First you create a master model file, which consists of sketches, planes, surfaces or other reference geometry. It is a good habit to avoid the use of solid bodies in the master model, because you are going to bring this model into each child part. Which could result in too many solid bodies. After your master model is finished, you use Insert Part to place this model in each child part. Based on the geometry in the master model, you can create the detailed child part.
Master model techniques create external references between the parent part and the children. These external references can be broken by improper file management practices. The most important rule to follow when working with parts that have external references is to NOT use Windows Explorer to rename or copy SOLIDWORKS files. Use SOLIDWORKS Explorer instead. Or use the SOLIDWORKS Explorer tools in the right-click menu of Windows Explorer, as in figure 3.
SOLIDWORKS Explorer can do the following:
We have seen how we can speed up the design process with the master model technique. The main advantage is the ability to perform rapid model changes, because you just need to change the master model and the child components will change accordingly. A nice bonus is the saving of assembly mates, when you are going to put the child components together. The master model already created the relative position for all the parts, so you don’t need any mates in the assembly.
Written by Martijn Visser, Elite Application Engineer
Categories: SOLIDWORKS, SOLIDWORKS 2017, Tips & Tricks, Usability