Creates a part file and derives the selected objects from the source part into the new part.
- Access
-
Ribbon:
Manage tab
Layout panel
Make Part
- Ribbon:
Sketch tab
Show Panel icon
. Select Layout panel to display the Layout panel.
Layout panel
Make Part
- Select one or more sketch blocks, solid bodies, or surface bodies and select Make Part from the context menu.
- Derive style
Derives a single, merged body without seams between planar faces.
Derives a single solid body with seams between planar faces.
Individual component appearances of planar faces are preserved.
Derives a single part that retains each component as an individual solid body. For example, an assembly with 20 parts derives to a part with 20 solid bodies.
Derives a single part with bodies as base surfaces.
- Status
Includes the selected objects in the derive operation.
Some child objects are included and some excluded.
Excludes the selected objects from the derive operation.
Represents the selected component in the derived part as a bounding box and creates a body from the bounding box shape. The reduced detail decreases memory consumption. The bounding box updates to reflect changes in the derived component or in the base component.
- Part information
- Part name. Enter the name of your new part.
Template. Select or browse to the part template from which the new part is created.
New file location. Enter or browse to the location where the new part is saved. Use to select a part that exists, if appropriate.
Default BOM structure. Select the bill of materials structure for the new part.
- Place part in target assembly
- Select to place the new part into an assembly. If this option is selected, the Make Part process will:
- Create a target assembly and insert your new part. The part is grounded at the assembly origin.
- Open the target assembly as the active window. The new part and target assembly are not automatically saved to disk. You save both when the target assembly is saved.
If this option is cleared, the Make Part process will:- Create a part file.
- Open the part file as the active window. The part file is not automatically saved. Save the new file.
- Assembly information
- Target assembly name Enter the name of your new assembly.
Template Select or browse to the assembly template from which the new assembly is created.
New file location Enter or browse to the location where the new assembly is saved. Use to select an assembly that exists, if appropriate.
Default BOM structure Select the bill of materials structure for the new assembly.
- Show all objects
- Select to show all derivable objects regardless of their Export status.
- Break link with base component
- Check the box not to retain link between the base component and the target part.
- Suppress link with base component
- Check the box to suppress link between the base component and the derived part or assembly.
Note: Not available when the Break link with base component box is checked.
- Link face color from source component
- Check the box to link the face color from the base component into the target part. If unchecked, the appearance is set to default appearance of the target part.
Note: A setting can be configured to default the Use color override from source component check box to remain checked or unchecked throughout your session. This check box can be accessed through the Application Options dialog box in the Part tab.
- Link sketch formatting from source component
- Check the box to link the face formatting from the base component into the target part.
- Link sheet metal styles
- Select check box to push the sheet metal thickness and other parameters to the derived body.
Note: Check this option to eliminate a mismatch between the part thickness and the defined sheet metal style thickness. If the sheet metal thickness does not match the thickness in the style definition, the derived part cannot be unfolded.
- Use oriented minimum bounding box
- Select check box to derive a solid body using oriented minimum bounding box.
- Scale factor
- Select or enter a scale factor to apply to the derived objects. The default value is 1.0.
Note: Selected sketch block definitions and their instances are scaled. The scale factor is appended to the block name to indicate the block was scaled.
- Mirror assembly
- Select to mirror the assembly. Specify the XY, XZ, or YZ origin work plane as the mirror plane.
Note: Sketch block instances of selected block definitions are mirrored. However, the block definitions are not mirrored.
- OK
-
Execute Make Part and close the dialog box. The target part and target assembly are not saved to disk. You save both when the target assembly is closed.
- Apply
-
Execute Make Part and keep open the dialog box. The target part and target assembly are saved to disk but neither are opened. The source part window remains open and the Make Part command remains active so you can continue to select different objects and create more parts.