{"id":193,"date":"2012-09-11T09:05:38","date_gmt":"2012-09-11T13:05:38","guid":{"rendered":"https:\/\/example.org\/cutting-all-ties-best-practices-for-removing-external-references"},"modified":"2013-11-21T10:59:02","modified_gmt":"2013-11-21T15:59:02","slug":"cutting-all-ties-best-practices-for-removing-external-references","status":"publish","type":"post","link":"https:\/\/blogs.solidworks.com\/solidworksblog\/2012\/09\/cutting-all-ties-best-practices-for-removing-external-references.html","title":{"rendered":"Cutting All Ties: Best Practices for Removing External References"},"content":{"rendered":"

Designing parts using the Top-Down assembly modeling technique can be extremely useful. If a component is designed with the \u201ctop-down\u201d technique, this means it is born in the assembly environment and it is designed using references to other parts within that assembly. Parts that are designed \u201ctop-down\u201d have the advantage of being able to update when related geometry in the assembly updates, much like features\u00a0 update in the part environment when other related features are changed.<\/p>\n

This can save a lot of time and hassle when it is a desired result, but it can also cost<\/em> a lot of time and hassle when it is not<\/em>. What happens when the User A wants to take a component that is designed \u201ctop-down\u201d and use it in an assembly other than the one it was originally designed in? User B may decide to adjust the original assembly and before you know it, User A has a part that has mysteriously changed shape so that it no longer meets their design intent. The key in preventing these undesired updates in \u201ctop-down\u201d designed parts is properly removing the external references that relate one part to another (or many others, for that matter).<\/p>\n

Step 1: Open the Part<\/strong>
\n<\/strong><\/p>\n

\"Before\"<\/a><\/p>\n

When you open a part that has been designed using the \u201ctop-down\u201d technique, you may notice that certain features and sketches in the design tree are appended by the notation \u201c->?\u201d This means that those specific features and sketches contain external references to a document that is
\nnot currently open. A feature that does not have external references may also display this notation if the sketch that is a parent to the feature does have external references. You can right click on any externally referencing feature and chose \u201cEdit In Context\u201d to open the assembly that this component references. You will notice once this assembly is opened, the notation next to these features and sketches change from \u201c->?\u201d to \u201c->\u201d.\u00a0\u00a0\u00a0\u00a0 <\/strong>
\n<\/strong><\/p>\n

\u00a0<\/strong> \"After\"<\/p>\n

 <\/p>\n

Step 2: Save the Part<\/strong><\/p>\n

If you are now planning on removing the external references to a part that was not originally your design, you should consider that the person\u00a0 who designed this component originally may still want the part to update in the context of their original assembly. It is best practice to use
\n\u201cSave As\u2026\u201d to save your version of the part. When you chose to \u201cSave As\u2026\u201d you will get a message saying you are about to replace the\u00a0 original document with the new one in the assembly unless you check \u201cSave as copy\u201d in the \u201cSave As\u2026\u201d dialogue. Please be sure to choose to \u201cSave as copy\u201d.<\/strong><\/p>\n

 <\/p>\n

Step 3: View the External References<\/strong><\/p>\n

You may wish to see a list of every external reference in the component. This can give you a good idea of what you need to adjust in order for
\nyour part to be \u201cfree\u201d to stand on its own. Simply right click on the part name in the feature tree and chose \u201cList External References\u201d in the drop down menu. A window similar to the one below will appear:<\/p>\n

\"Step<\/a><\/p>\n

This window can provide you with detailed information on every external reference in the model. It also provides you with the options to \u201cBreak
\nAll\u201d, \u201cLock All\u201d and \u201cUnlock All\u201d. These options can be used as an alternative to removing the references manually. \u201cLock All\u201d locks or freezes the references until they are unlocked at a later date. This means that changes to the original assembly will not affect this new component. It is fully reversible by choosing to \u201cUnlock All\u201d. However, it does not make adjusting geometry an easy task because much of the geometry may still be tied into the original assembly. \u201cBreak All\u201d will blindly break these references, and it is NOT recommended in any circumstance.<\/strong><\/p>\n

\u00a0\u00a0<\/strong><\/p>\n

Step 4: Removing the External References\"Step<\/a><\/strong><\/p>\n

It is finally time to actually purge the model of all these external references. This can be a tedious process, depending on how much of the model is dependent on its parent assembly. The key is to start with the latest change and work your way up the feature tree to the oldest changes. Working from the bottom up in the Feature Manager helps prevent rebuild errors.<\/p>\n

Most of the external references are likely to reside in the sketch environment. These references will be in the form of relations and dimensions created to the geometry of other parts in the original assembly. These relations and dimensions must be deleted so that the sketch geometry can be redefined internally. Below is an example of a sketch that was created using \u201cConvert Edges\u201d. These edges no longer exist, so the \u201cOn Edge\u201d relation must be replaced.<\/p>\n

Any easy way to do this is to use the \u201cDisplay\/Delete Relations\u201d dialogue. Through this dialogue, it is easy to delete all relations, leaving the
\nsketch completely under undefined:<\/p>\n

\\\"\"<\/a><\/p>\n

A simple sketch like this one can be fully defined with only a few relations and dimensions, however it may be more difficult to constrain a sketch with more complicated geometry. The following sketch shows how this can be easily accomplished: \"\"<\/a><\/p>\n

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This sketch has \u201cOn Edge\u201d and co-linear relations to another part. You may also notice that there are some dimensions that don\u2019t seem to point to any edges. This is because these edges exist in another model. These are all references that need to be removed and replaced. You can easily get rid of these relations by choosing to delete all relations in the \u201cDisplay\/Delete Relations\u201d dialogue, however, that would also result in
\nthe deletion of a number of internal relations in this sketch. If you don\u2019t wish to take a chain saw to the entire sketch, but want a fast and easy way of deleting the unwanted relationships, there is a filter in the \u201cDisplay\/Delete Relations\u201d tool to only view external references. From here you can easily delete ONLY the external references and maintain the rest: \"\"<\/a><\/p>\n

You can see that all of the symmetry relations are maintained as well as the dimensions that do not reference another components geometry. This sketch is still very much under defined, so another tool that can be used is \u201cFully Define Sketch\u201d. This tool allows you to select relations you\u2019d like SolidWorks to look for in the sketch. It also allows you to define a base point or base line for SolidWorks to dimension the sketch to. Once these selections are made, you may get the following message:<\/p>\n

\"\"<\/a><\/p>\n

This means the geometry itself is fully defined, but the location is not. The easiest way to get a fully defined sketch at this point is to dimension your geometry to the origin of the part.<\/p>\n

 <\/p>\n

\"\"<\/a><\/p>\n

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In the end, you want your feature manager tree to look something like this. You\u2019ll notice, all of those pesky notations from before (\u201c->?\u201d and \u201c->\u201d) are gone, showing that you part is all grown up \u2013 it can now survive on its own, independent of the assembly it was born in! There are many other techniques that may be used for freeing a part from its external references. Apart from the sketch environment, sketch planes can be edited so that only internal planes are referenced and extruded features can be edited so that geometry from other parts isn\u2019t used for \u201coffset\u201d or \u201cup to\u201d start and end conditions. All of these techniques (and more) are taught in our Advanced Assembly class. For more information on classes, click here<\/a>.<\/p>\n

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