What is Master Modelling?
'Master modelling' is a CAD modelling technique where models are created in relation or reference to another, separate model file.
Consider a plastic part that is to be injection moulded; the finished part geometry can be inserted into another part file and the geometry for the tooling built up around it.
If any changes are made to the original, inserted part, then the downstream features will update accordingly. Using the main body as a reference will ensure the shape and fit is correct.
Within SOLIDWORKS, master modelling can be utilised in both part and assembly environments. We'll be focused on just the part modelling environment in this article.
Who uses Master Modelling Techniques?
Master modelling is commonly used in the consumer products industry, but it isn't limited to any single industry or designer.
You'll find that master modelling can be applied to many different types of product design in SOLIDWORKS, and its advantageous to consider whether your models will benefit from using it.
Let's consider an example with a simple consumer electrical product like an electric shaver.
The main body may be used as the inserted master part to provide positional references and drive the design, allowing other items (such as button details or the razor mount) to be designed. Using the main body as a reference will ensure the shape and fit is correct.
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Working with Master Models
How to Create a Master Model in SOLIDWORKS
We'll start with a blank SOLIDWORKS part file. To begin modelling, we need to insert a part into another part environment to create a parent and child linkage between the files.
To insert a part, simply use the Insert > Part menu string:
When inserting, you will be asked what data you want to bring along. Choose the check boxes as needed.
If you forget to pick an option, you can always edit the feature later and choose different options.
How to Check External References in SOLIDWORKS Parts
If you have received a model with an inserted part and are worried that you don't see the latest information, then you can check in on the references.
The Feature Manager Tree will show a symbol attached to the inserted part. There are four possible symbols:
-> External reference intact and up to date- the master model is open in the background.
->? The reference is out of context, and this may be because the master model is not open or cannot be found.
->* The reference has been locked to prevent changes from propagating- locked references can be unlocked.
->x The reference has been broken preventing changes- and this is irreversible.
If you wish to interrogate further, you can right click the inserted part and choose External References from the right-click menu. This reveals a dialogue showing you the expected location and name of the inserted part, and details about any links.
How to Replace 'Driving' Master Model Parts in SOLIDWORKS
As the new part file has a reference back to the inserted master model so any changes made to the geometry or metadata of the inserted model will propagate through.
So what if we want to replace the master part with an alternative component or file? How can we do this without breaking our references in the new part and impacting the driven features?
Master modelling is an example of multi-body part modelling, as it is utilised within the part environment rather than within an assembly.
Weldment structures in SOLIDWORKS are based on multi-body part modelling, where timber and steel frames and other structures can be created from a master sketch. Modifying the master sketch will automatically update the solid bodies!
The answer isn't obvious and must be done before opening the file. We need to swap out the file and change the reference before SOLIDWORKS notices.
To change a reference when opening a file in SOLIDWORKS, look for 'References' button in the File > Open dialog box. Click once on the file you want to open, and then click the References button.
This displays all the external references within the file. In this case, we're interested in the file location of the inserted part - our master model.
Within this dialog, we can double click on file and locate a substitute part. If you've attended our SOLIDWORKS Essentials or Advanced Part Modelling training courses, then you'll probably notice that this is the same way that you can replace part references in the assembly and drawing views.
This will then replace the part, but be aware that you may find that some downstream features develop warnings or errors that can be resolved by repairing and editing sketches or features to re-aligned them with the replacement part.
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