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Exporting Multi-body Parts to an Assembly

Thursday April 10, 2014 at 10:29am
The multibody part environment is a huge strength of SOLIDWORKS- the diverse range of features we provide in the part mode, means that you can gain fully detailed designs without having to even explore the assembly mode- there may be examples where you wish to convert multibodies to assemblies though- for example: Animations; assigning part numbers; assembly specific features. In this blog we explore some of the ways to do this.
1- Insert into New Part
This option allows you to take one, or more of the solid bodies in your part mode and directly export into a new single part environment- it retains its reference to the main origin location, so you can then put this into an assembly to build the structure back up. The advantage of this feature is that there is an external reference back to the parent model in the form of a Stock feature- as such the new file won't have feature history, but will alter if the parent model changes. The reference is only one directional though- additions to the newly derived part will not change the parent- ensuring this stays preserved. The feature tree displays this reference using the symbol ->. You can find this feature by right clicking on a body under the Solid Bodies folder.
2- Save Bodies
This command is particularly useful if you want to save all bodies, with each being taken into a new file and have an assembly created at the same time. In preparation for this it is worthwhile renaming the bodies (under the Solid Bodies folder- F2 to rename) as this is the default name taken to save the file, therefore this will save you a bit of time. The feature can be found via Insert > Features > Save Bodies.
Within the command you can choose which bodies you want to export by checking the tick boxes, then there is a button to "Create Assembly" this will then save the bodies as parts, and remate them into an assembly by positioning the parts relative to the assembly origin- so they slot in at the correct place. The external reference back to the original master model reacts a little differently in this case- as the Save Bodies command is shown as a feature in the tree, therefore having a historical position. This means that any changes to features before the Save Body operation will alter the derived parts, but additional features after the Save Body command will not propagate through- hence you may wish to use Save Bodies at the end of the design, or use the roll back bar to reorder features. The example image underneath shows that you can use this command to create sub assemblies- of the CD tower on the desk.
And this is what you are left with:
By Alex Hall
Applications Engineer

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