What is a Multi-Body part in SolidWorks?
In SolidWorks, a part document (.sldprt) can contain multiple bodies. These bodies can either be solids, surfaces, or graphics. A Multi-Body part file is one that contains more than one solid body. If a part file has only multiple Surface bodies it is not considered a multi-body part. Graphical bodies have very limited usability in SolidWorks hence these are also not considered as a Multi-Body part.
How do I know if a part file is multi-body?
A folder named Solid Bodies along with the number of Solid Bodies present in a part document appears in the FeatureManager design tree. You can expand the folder to see the list of all the solid bodies. You can right-click on any of the bodies to rename them according to your choice (by default the name of the body will be the last feature performed on that body). You can hide/show them or change their transparencies. You can do exploded views. You can assign them different materials and appearances.
What is the difference between a MultiBody part file and an assembly?
A multi-body part consists of multiple solid bodies that are not dynamic i.e. you can’t move them around, while an assembly is used to represent dynamic motion among bodies. Hence, multi-body parts cannot be used instead of assemblies.
Also, tools such as Move Component, Dynamic Clearance, and Collision Detection are available only with assembly documents. A Multi-body part file can be shared directly but you can’t share an assembly file without the part files that were used to create the assembly in the first place.
Why and when should I create a multibody part file?
There are several reasons why you may want to create a multibody part. Some are listed down below:
1. It is easier to use the Pattern/Mirror command of bodies: More often than not we find ourselves to be modeling a part that is either entirely symmetric or has some symmetry or some type of pattern in it. Symmetry modeling not only simplifies the creation of axis-symmetric parts and saves huge time but it also speeds up performance for these types of parts.
While you can apply a symmetry of features to achieve the result, you may sometimes find that the pattern/mirror will fail just because of the way those features have been added. Or sometimes you may find yourself in a situation where you need to make a pattern/mirror of a huge number of features. So what you can do instead of making a pattern/mirror of features, is to make a pattern/mirror of bodies.
Take a look at the below part for example. This is the body of a Tank. It is symmetrical along the right plane. So what we did is we only modeled the right side of the part. Now we are going to apply the Mirror tool. Obviously, we can’t apply a mirror of features as it took us more than a thousand features to model the right side. So what we are going to do is to make a mirror of all the bodies.
To make a pattern/mirror of bodies click on the Bodies option present in the PropertyManager of that tool and then select all the bodies you want to pattern/mirror. Use box selection if there are a lot of bodies. While mirroring bodies you can also select the Merge solids option and then specify the Feature scope (explained below) to make the new body combine with the old one.
For Patterns, you can use the Combine tool (as many times as you like) available in the Direct Editing Tab or go to Insert-> Features -> Combine to combine multiple overlapping/coincident solid bodies into one.
2. Shell can only be applied to solid bodies and not on features: Let’s say you have a solid body that is already shelled and now you have to add a shape that is to be shelled with the same thickness. Since you have already added a shell feature to the body you can’t add this feature again with the same thickness. So what you can do instead is to make that shape as a separate body, apply a shell on it and then combine or bridge it with the existing body.
3. To convert to a mesh body: Sometimes you may want to convert a solid body into a mesh body, let’s say to convert a 3D texture into 3D model detail. And since there is very little you can do with a mesh body in SolidWorks you don’t want to convert the whole part to mesh. So instead of modeling the part as a single body, model the area on which you want to add the 3D texture as a different body which you can then later convert to a mesh body without affecting the other bodies.
4. Weldments and Sheet Metal: Weldments and sheet metal work with the multi-body part. Weldments and sheet metal tools are used for modeling frames, sheet metal products, and fabrications in general. If you have used Sheet Metal tools or Weldments you may find that there is no Solid Bodies folder present in the feature tree. Instead, there will be a Cut List folder that will list all the different solid bodies.
5. To make Molds: More often than not we have to break our part into multiple pieces so that it can be mass-produced using molds, etc.
6. Design Requirements: Let’s say you need to design a spoked wheel and you know the requirements of the rim and the axle. However, you do not know how to design the spoke. With multibody parts, you can create the rim and axle, then create the spoke to connect the bodies.
7. To apply different materials: If you want to apply different materials in a single-part document you have to create a multi-body part file. You can then assign different materials to different solid bodies by right-clicking on the solid body from the Solid Bodies folder and clicking on Material to add any sort of material that you like.
You can also add different appearances to each and every solid body as per your liking.
9. To create exploded view of a Part: An exploded view in a multi-body part shows how the solid bodies will be assembled. In an exploded view the solid bodies spread out and are positioned to show how they fit together. You create exploded views by selecting the Exploded View tool from the Insert menu and then dragging solid bodies in the graphics area, creating one or more explode steps. Read More…
10. To create assembly directly from the part file or to save different bodies of a Multi-Body part file separately: You can use a Multi-body part file to automatically create an assembly file that will contain all the solid bodies in it arranged in the same way as they are in your part file. These bodies will be fixed in place but you can float them and then add any mates if required. This is very useful when making complex designs or when preparing part files for molds. Go to Insert -> Features -> Save Bodies or right-click on the Solid Bodies folder and select Save Bodies.
11. Allows you to perform boolean operations for making complex model geometry: You can use the boolean operations such as adding multiple bodies, subtracting bodies from one another, or keeping only the common part of the bodies. You can access these boolean operations using the Combine tool present in the Direct-Editing toolbar or go to Insert -> Features -> Combine.
12. All bodies in a Multi-Body part file are present inside one file: This makes sending and managing files easier and more convenient.
And there are many more reasons why you should make a Multi-Body part file. Listing them all is beyond the scope of this article.
How to create a MultiBody part file?
You can create multiple solid bodies in a single file with the help of the following methods:
1. By using Boss/Base and Cut commands:
- Extruded Boss/Base and Cut
- Revolved Boss/Base and Cut
- Swept Boss/Base and Cut
- Lofted Boss/Base and Cut
- Boundary Boss/Base and Cut
While using the Boss/Base mode of these tools to model your geometry you have the option of Merge results (this option is only available when there is at least one solid body present already). If you uncheck this option you will find that the geometry that has been created by the feature is not merged with the existing body and is now created as an individual body.
And you can also use the cut mode of these tools to cut your single body into multiple bodies. If your cut does results in creating multiple bodies you will get a popup window asking you which bodies you want to keep.
2. By using surface tools:
- Converting Surface Bodies to Solid Bodies: If your part file contains surfaces and you decide to convert them into solid bodies, you may find yourself with multiple solid bodies. Read more.
- Cut with Surface: Read More…
- Thicken and Thickened Cut: Read More…
3. By using the Split command:
This tool is extensively used to split a single body into multiple bodies. Go to Insert -> Features -> Split or select the Split tool present in the Direct Editing toolbar. Read More…
4. By inserting an existing part:
Insert Part command present in the Insert menu is used to insert an existing part file into another part file. In multibody parts, you can precisely place bodies using mates. Mates such as Coincident, Angle, Parallel, Perpendicular, Concentric, Tangent, and Distance are available.
When you insert a part into an existing part file, mate references, if present, in the inserted part are used automatically to place the inserted part. You can also apply mates:
- While inserting a body into a part, select the Locate part with the Move/Copy feature in the Insert Part PropertyManager, or
- If the body is already in the part, use the Move/Copy Bodies tool present in the Direct Editing toolbar or go to Insert -> Features -> Move/Copy.
Then select the Body that you inserted in the Bodies to Move/Copy box and then click on the Constraints button to add as many mates as you want or use Translate/Rotate button to manually position the body.
5. By saving an assembly as a multi-body part document:
Saving a complex assembly as a part file can be useful in various situations. Like if you want to scale a complete assembly. Or when you want to share your assembly but don’t want to risk design integrity by sending each and every internal detail. So instead you can select a few of the outermost components to be included in the part file which in turn also reduces the size of the part file.
To save an assembly as a multi-body part document:
- Open an assembly document.
- Click .
- Set the Save as type to Part (*.PRT, *.SLDPRT).
- Select one of the following:
- All Components: This option saves all components as Solid Bodies. (Tip: Components that are hidden or suppressed are not saved).
- Exterior Faces: This option only saves the exterior faces of the assembly as Surface Bodies. No solid bodies are saved.
- Include specified components: This allows you to save the visible components as Solid Bodies.
- Select or clear the following:
- Preserve geometry references: If checked, this will save all the assembly mates in the multi-body part. This is useful when you use the multi-body part as a simplified representation of the assembly in a higher layout assembly and then make changes later. When you change the subassembly and then save the subassembly again as a multi-body part, you can replace the previous multi-body part with the new multi-body part, without having to recreate the mates.
- Click Save.
What is the Feature Scope?
When you are working on a multi-body part, for some features, you will see that there is a Feature scope option present at the very bottom of the PropertyManager. Feature scope is a very useful option and it is very crucial that you master it if you want to work on a multi-body part file.
Tip: If there is no Feature Scope present during a Boss/Bass feature make sure that the Merge Bodies/Merge Result option is checked in the feature’s PropertyManager.
Feature scope is used to specify which bodies will be affected by the feature you are creating. There are 2 options available under the Feature Scope menu.
- All bodies: If selected the feature will be applied to all the existing bodies every time the feature regenerates. For example, if you are performing a Cut Extrude on a multi-body part with this option selected, it will cut all the bodies that are intersected by the end conditions of the cut.
Notice how all 4 of the squares are cut by the Cut-Extrude tool. All Bodies option regenerates the entire model, hence sometimes it is a bit slower.
If you are using a Boss/Base Feature, this option will merge all the bodies that are being touched by that feature. For example, if we were to perform a Boss Extrude instead of Cut in the above example, the Boss-Extrude feature will create a cylinder while merging all 4 squares with it and leaving us with only one solid body.
- Selected bodies: If selected, the feature will only be applied to the bodies you select.
Auto-select: At the time of creation, the feature automatically detects all the intersecting bodies and selects them for you. Auto-select is faster than All bodies because it processes only the bodies on the initial list and does not regenerate the entire model. If you want to manually select the bodies that you want the feature to affect then you have to clear the Auto-select option.
Solid Bodies to Affect: You can manually select the bodies in the graphics area that are going to be affected by the feature and those bodies will be highlighted in green.
Notice in the final image below how the Cut-Extrude feature cuts only the two squares that we selected and left the other two as they were.
If we were to create a Boss-Extrude in this example, the cylinder will only be merged with the two squares we selected and we will have a total of 3 solid bodies.
Note: If you use the rollback bar to add new bodies to the model before the feature, that is intersected by the feature, you need to use Edit Feature to edit the extrude feature, select those bodies, and add them to the list of selected bodies. If you do not add the new bodies to the list of selected bodies, they will not be affected by this feature.
Tip: Most beginners do not pay attention to the Feature Scope while adding features and then they end up with either more or less solid bodies. So if you are working on a multi-body part make sure to define this option every time you make a new feature that requires Feature Scope and keep an eye out for the number of solid bodies you have in your part file.
And that’s it. We hope that this article provided you with all the important information you needed to work on a multi-body file in SolidWorks.