When working in a CATProduct document, it is no longer necessary to copy and paste the bodies belonging to distinct parts before associating them. You can directly associate these bodies using the same procedure as described in this task.
Structuring Your Design
Generally speaking, using Boolean Operations is a good way of structuring your part. Prior to designing, you can actually define the part's structure by associating a body containing geometry with empty bodies. Once these specifications are done, you can then concentrate on the geometry.
In this page, you will find the following information:
-
This is your initial data: the Add part is composed of three bodies. Each body includes a pad. These pads are therefore independent. To add Body.1 to Part Body, select Body.1.
- Adding a set of bodies (multi-selected via the Ctrl key) is possible. This capability will increase your productivity.
-
Click Add
.
The Add dialog box that appears displays the name of the selected body, the Part Body and the feature after which the Add feature is to be added.
By default, the application proposes to add the selected body to Part Body. For the purpose of our scenario, we keep this location. Note however that you could add Body.1 to Body.2 one just by selecting Body.2.
From V5R15 onward, you can get an idea of the result just by clicking the Preview button.
-
Click OK.
The specification tree and Part Body now looks like this:
You will note that:- the material common to Part Body and Body.1 has been unified
- both pads keep their original colors.
-
Double-click Add.1 to edit the Boolean operation.
The Add dialog box is displayed. -
Select Body.2 from the specification tree or from the geometry area.
PartBody and Body.2 are associated. The material common to Part Body and Body.2 is retrieved.
Bodies You Can Use
-
Performing a Boolean operation using a set of bodies (multi-selected via the Ctrl key) is possible unless the bodies are located in ordered geometrical sets. This capability will increase your productivity.
- Adding a body to a solid body and vice versa is possible. In that case, the second body you select remains at the same location in the specification tree once the Boolean operation is done. For reference information, refer to Mixed Boolean Operations.
-
From V5R16 onward, you can add a body set in an ordered geometrical set (OGS) to another body set in the same ordered geometrical set or in a distinct one. Note that the different Boolean operations can be performed using dedicated contextual commands.
Depending on whether the Boolean operation interrupts the sequential construction of the geometry or not, the application behaves differently.No interruption of the sequential construction of the geometry
If there is no interruption of the sequential construction of the geometry, two cases are to be considered:
- if the bodies are set in the same OGS, the operation is performed and the second body selected is located below the Boolean operation node.
- if the bodies are set in distinct OGS, the operation is performed and the second body selected is moved below the Boolean operation node.
Interruption of the sequential construction of the geometry
If there is an interruption of the sequential construction of the geometry, two cases are to be considered:
- if the bodies are set in the same OGS, a warning message is issued informing you that the operation is going to be canceled: breaking the sequential construction of the geometry is not allowed when the operands belong the the same OGS.
- if the bodies are set in distinct OGS, a warning message is issued letting you choose between canceling the operation or going on. If you decide to continue, the second body you selected remains at its initial location in the tree.
Location of Bodies Once the Boolean Operation is Complete
Once a Boolean operation is done, the second body you selected is moved below the Boolean operation, as illustrated in the scenario above. However, there are exceptions to that rule:
-
Adding a body to a solid body and vice versa is possible. In that case, the second body you select remains at the same location in the specification tree once the Boolean operation is done. To see an example, refer to Mixed Boolean Operations.
-
If adding bodies results in an interruption of the sequential construction of the geometry, the second body you selected to perform the Boolean operation remains at its initial location in the tree when the operation is complete. To see an example, refer to the Location of Bodies Once the Boolean Operation is Complete paragraph of Assembling Bodies.
Notes
- You cannot re-apply the Assemble, Add, Trim, Intersect, Remove and Remove Lump commands to bodies already associated to other bodies. However, if you copy and paste the result of such operations elsewhere in the tree you can then use these commands.
-
Avoid using input elements that are tangent to each other since this may result in geometric instabilities in the tangency zone.
Optimizing Your Design
The Only Current Body option
displays
only the features of the current body and greatly improves the application
performance whenever you edit these features. For more information, refer
to
Display in Geometry Area.
Interrupting Boolean Operations Computations
In case you made a mistake when performing a Boolean operation, you can
interrupt the computation launched after clicking OK, provided
that the computation requires at least 5 seconds to perform.
When a computation exceeds 5 seconds, a progress bar appears and provides a
Cancel option. To interrupt the operation, just click that
Cancel button. This interrupts the process and then displays an
Update Diagnosis dialog box enabling you to edit, deactivate, isolate or
even delete the Boolean operation in progress.
This capability is available for any types of Boolean operations you are creating or editing.
Colors
When performing a mixed Boolean operation, the resulting geometry inherits the color of the first geometric entity selected.
