Last week, I introduced you to making derived sketches to save time in duplicating features on your part. Today is all about using the Insert Part command to create a derived part. A derived part is an extremely useful technique for adding features to a part without affecting the original part.  When the original part is updated the derived part is updated as well. There a many reasons you may need to use this technique in your usage of SolidWorks. I have seen it used by molders to prepare a model by adding drafts, splits and modifying faces for making the mold tool. I use this technique when I have a purchased part in my design library that I need to make modifications without actually affecting the geometry of the original part.

Today’s example will be making modifications to a purchased die set that can be purchased from many vendors. If you aren’t familiar with die sets, they are handy kits that usually contain a couple of pre-machined plates, shafts and bushings. They are a great time saver when you create tooling for a variety of uses.

Inserting a Part

To start off, open a new part in SolidWorks. From the Insert menu, select Part.

In the Open window, select the part that the new part will be derived from.

A representation of the referenced part will be shown in you graphics area.

In the Insert Part PropertyManager, you can select the elements of the original part you want to transfer into the derived part. You can add as few or as many elements but I tend to go with the minimalist approach and transfer only what I know I will be using at a later time. At this point you can select the Launch Move dialog option in the Locate Part section to locate the inserted parts in relation to existing sketches or part geometry. Since this is the first feature we are adding to the part, click the green check mark and the part will be inserted in the orientation it exists in the original part.

You will now see the part shown as a feature in the FeatureManager followed by a arrow (->) this designates that the feature has an external reference.

Expanding the feature will show you the elements you selected to be transferred into the new part.

Locating Inserted Part

We will be covering locating a part in the future when we discuss multibody parts but I wanted to show you the Locate Part command. If you select the Launch move dialog…

…you will be presented with a PropertyManager that same basic mates used in assemblies to locate your solidbodies.

Add Features to Inserted Part

Once the referenced part has been inserted into your derived part it becomes a solidbody. You can add features to the part just like any other solidbody but you cannot not modify any of the existing features of the referenced part. In this example, I wish to add a series of holes that will be used as mounting for another part.

You will see in the FeatureManager, that the holes I added are a new feature in the derived part and the original solidbody has not been changed.

Breaking Link to Referenced Part

As I mentioned, you cannot modify the features of the referenced part. If you needed to make a change to the parent part, you must modify it separately but understand that any changes made to the parent part will be reflected on all of the derived parts made from the parent part. If you need to modify the features of the part only in your current model and you do not wish to affect any more of your parts; you can break the link to the parent and transfer the model information into you current model. To do this right-click the feature in your FeatureManager and select List External Refs.

In the External References window you will see the external references to the part part listed, as well as any other external references you may have created in you part.

In SolidWorks 2008, a new option was added that allows you to insert the features from the parent part when the references are broken. Select Insert the features of original part(s) if references are broken.

Then click the Break All button.

You will be prompted with a message warning you about breaking the references and how you will not be able to undo the action. Select OK.

The external references list will now be clear and the features from the original part will be inserted into your FeatureManager under a new folder that contains the name of the original part. You can leave the features in the folder or delete the folder if you prefer it.

In addition to breaking the links after the part is inserted you can also choose to break the link when the part is inserted by selecting Break link to original part in the Insert Part PropertyManager.

This can be buggy at times

Just a warning about breaking the links to the original part. I have found that in SolidWorks 2008 that sometimes SolidWorks will crash when you try to break the link to some parts. In fact, in writing this article I was unable to break the link to my part without my SolidWorks crashing on two separate computers, that is why I do not show the FeatureManager after the part link is broken. I have not had the opportunity to test this out in SolidWorks 2009 yet and I hope that it has been addressed. Let me know what you experiences are with breaking the link to external parts.

More to Come…

That does it for today’s introduction to inserting parts to make derived parts. Soon we will be looking at the other two types of Derived Parts: Mirror Part and Derived Component Part so make sure you subscribe to my RSS feed so you don’t miss anything. Ciao!

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