Insert Part for Multibody Modeling in SOLIDWORKS
Top down or “in-context” design is a contentious area of modeling for many SOLIDWORKS CAD users. Careless in-context references can result in a web of dependencies between files that can lead to a variety of problems.
The Insert Part feature provides a simple alternative to traditional assembly in-context editing and can be used for both simple and complex use cases.
This article will outline two case studies: the simple case of designing one part around another purchased or mating part and the more complex case of utilizing data from a master model.
Case Study 1: Designing Around Metal Insert
In this example, a metal threaded stud will be inserted into a molded plastic knob to allow subtracting the material necessary to produce the overmolded part.
The Insert Part command, visible in Figure 1 below, can be found on the “Insert” drop-down toolbar when an existing part file is already open.
Figure 1. Insert Part feature under the Insert pull down menu.
The part file to be inserted is browsed for and a particular configuration can be chosen.
One valuable feature of the Insert Part tool is the ability to specify which data gets transferred. This can include solid and surface bodies, sketches, planes and other reference geometry as well as material data and certain properties.
Choosing to transfer only the data that is needed will help keep the part model organized.
The Insert Part feature that gets added to the model tree can always be edited later to transfer more information or to update the configuration of the inserted part file.
Figure 2. Insert Part options and preview.
By default, the inserted part is linked to the original via an external file reference, unless the option “Break link to original part” is selected.
Positioning the Inserted Model
If the model to be inserted has the appropriate position about its origin, then no extra work is necessary. The checkmark can be clicked to insert the part with its origin aligned with the base part’s origin.
Most of the time, however, the inserted part will require positioning. There are two options to choose from if the “Locate part with Move/Copy feature” is selected. Enabling this option launches a prompt similar to the Move/Copy body feature which has two modes of operation.
Visible in Figure 3 below is the first mode which allows specifying either a translation or rotation in X/Y/Z coordinates allowing for a finite offset. In this mode, translation and rotation must be applied separately, which means it may be necessary to use a second manually defined Move/Copy body feature to achieve the desired result.
Figure 3. Locate Part with translate/rotate option.
The “Constraints” option in the Locate Part tool is visible in Figure 4 below. This option functions similarly to assembly-level mating and allows creation of multiple mates to locate the inserted part within a single prompt.
Figure 4. Locate Part with constraints option.
Referencing Inserted Bodies
A valuable addition in more recent versions of SOLIDWORKS is the ability to perform Interference Detection on multibody parts which can be seen in Figure 5 below:
Figure 5. Multibody interference detection.
Now that the interference is clearly visible, any part or multibody modeling techniques can be used to correct it.
Traditional sketch-based features such as extrude cut or revolved cut can be used along with Feature Scope to selectively target only the base model, as shown in Figure 6.
Figure 6. Sketch based features with feature scope.
One of the benefits of having both bodies in one file, however, is the ability to use Boolean-style modeling operations such as the Combine or Intersect features.
Figure 7 below shows the setup required for subtracting the insert from the base part using a Boolean-style modeling command.
Figure 7. Subtracting inserted body.
This approach should ensure the plastic part always updates correctly to subsequent model revisions. In comparison, the sketch-based methods may break or require editing if the profile is substantially altered in the inserted file.
Figure 8 shows the result of the subtract operation. Note that in the process of subtracting, the inserted body is consumed.
If it is desired to keep the inserted body in the final model, the body can be copied beforehand with a Move/Copy body feature and the “Copy” option enabled.
It is important to be conscious of the file references occurring behind the scenes when using any form of in-context modeling.
File references can be viewed by right clicking the Insert part feature from the tree and selecting “External References…”
Figure 8. Final result and accessing file reference.
While the ability to have the part file automatically updated when the source inserted file changes can be of great value during the early stages in the design, there may be times when you need to lock the design to prevent further changes.
The “Lock All” option is useful in this case, as it will temporarily lock the reference until further notice, preventing the inserted file from changing unless it is unlocked.
If it is necessary to break the link from the inserted file permanently, the “Break All” option can be used combined with the checkbox to include original features, as shown in Figure 9 below.
Figure 9. Break All references and Insert features.
This action is irreversible, and in some cases the inserted features may have sketch or relation errors that need to be corrected, so it is best to create a backup of your file before performing this operation.
Figure 10. Inserted Features after using Break All option.
The results are the features from the inserted part being grouped in a folder neatly within the original part model with model intelligence allowing for straightforward edits.
This case study is also available in the form of the video tutorial SOLIDWORKS: Insert Part Feature for Multibody Part Modeling.
Case Study 2: Master Model Workflow with Insert Part
Product designs featuring complex shapes with multiple mating components, such as cast or molded enclosures, can also benefit from the Insert Part feature when used as part of a master model workflow.
Figure 11. Master model of enclosure – single solid body.
In this workflow the master model is constructed either as a set of solid bodies, surface bodies or a hybrid of the two. Figure 11 above shows a solid body that represents the drafted halves of a multi-piece enclosure as well as a surface to represent the parting line and some additional sketches that contain information that may need to be shared between pieces of the enclosure.
The goal of the master model is to capture only enough to define the overall form and the mating features of the split. New part files are created, and this base or “master” model is inserted into them using the Insert Part feature.
This first part file will represent the top of the enclosure, so a surface cut feature is used to discard the material below the parting line. Further detailing is performed on top of the inserted body until this part is complete.
Figure 12. Detailing top of enclosure – Insert Part feature is first in tree.
This process is repeated for other part splits. A new part file is created, the master model inserted, the part is cut down to the desired split piece and then detailed.
Splitting up a complex model using a master model workflow has two major benefits: reducing the feature complexity and rebuild time in any one file and allowing multiple designers to work on different portions of the design simultaneously.
As the Insert Part feature maintains an active reference to the base master model part, any changes to overall dimensions or the form of the enclosure will update and propagate through the “child” split parts.
The detailed parts are then put together in an assembly for final validation and accurate bill of materials.
Figure 13. Assembly of individual detailed parts.
Beware Out of Context
A final note of caution with file references: Be careful of loading the part out of context. In SOLIDWORKS, this is symbolized by a question mark ( ? ) next to the inserted file name.
The question mark is easy to overlook. Look hard for it because it indicates that the referenced file has not been loaded, meaning changes will not be reflected in the model. It can be resolved manually by opening the selected file or right clicking and choosing “Edit in context.”
Figure 14. Out of Context indicator in System Options.
To manage this in a more automated fashion, System Options for External References (visible in Figure 14 above) can enable automatically loading referenced documents or prompting on each load.
Insert Part Versus Other Methods
Insert Part has many strengths when only one other part file needs to be referenced, as in the case of the metal insert shown in the first example and in the master model workflow shown in the second.
If a part needs to draw references and information from multiple different part files, then in-context assembly references are a much more obvious choice.
Nesting inserted parts multiple layers deep should also generally be avoided due to the difficulty of diagnosing file reference issues if they were to occur.
For the master model workflow specifically, there are other methods available within SOLIDWORKS such as the Save Bodies feature that could also be explored. Most other methods require less initial work upfront but may also have less flexibility.
When compared to Save Bodies, a benefit of Insert Part for master models is the ability to carry over sketch and reference geometry information rather than just the body data, as well as the ability to insert features when breaking references.
Although Insert Part allows choosing the type of data to transfer, such as planes and bodies, it does not allow isolating specific data. This can be a potential benefit for assembly in-context relation, in the event there is an abundance of sketch or body information as only the data needed for a particular file can be referenced in.
This article outlined two case studies for use cases of the Insert Part feature in SOLIDWORKS. For simple multibody needs such as referencing geometry of another part file, the Insert Part feature can help avoid many of the pitfalls and complexities of assembly in-context references. For “master model” workflows, the Insert Part command differentiates itself by allowing propagation of reference geometry and sketches to derived or child models.
In general, SOLIDWORKS provides a variety of means of achieving the same end result and its important to explore them to find the one that works best for your application. Hopefully this article will inspire you to explore the Insert Part feature the next time you need to reference another part file.
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