Revolved Solids (3-D)

3-D Standard > New > Revolved

Revolved solids are created from sketches by cloning and rotating them about an axis lying in the screen plane.

On activating this function, the New revolved solid dialogue window is displayed.

Recommended procedure:

1. Enter the Article number.
2. Activate the Referenced checkbox if you want the revolved solid to be referenced.
3. Activate the Feature checkbox if you want a corresponding feature of this revolved solid to be included in the feature log.
4. Activate the BOM-relevant checkbox in order to automatically assign this attribute to the created revolved part.
5. Choose theType. Revolved solids can be created as entire bodies or segments.
6. Enter the Start angle and End angle for segments.
7. Under Sketch for cross-section, choose the type of cross-section definition. You can create a new sketch or use a sketch that already exists in the drawing.
8. Specify the Rotation axis.
9. If you first want to check what the created part looks like, click the Preview button, followed by Apply if you want the part to be created as displayed. If you want the part to be created directly – without a preview –, click Create.

The revolved part will be inserted as main part into the drawing.

Revolved solid - as segment and and complete body, (1) Sketch, (2) Rotation axis

Please also read the notes on the purposes and representation of sketches.

Please note:

• If you want to insert the revolved part as sub-part to the active part, click and select Create new revolved solid, as sub part.
• It is recommended to apply the Sort GE (sketch) function to sketches first.
• Internal cycles, i.e. closed polylines, circles and ellipses lying within a sketch area, are interpreted as cut-outs/bores.
• Circular cross-sections produce toruses.
• Revolved bodies can only be created as analytical bodies. Ellipses and ellipse arcs are exceptions.
• The rotation axis must not intersect the sketch and always lies in the screen plane.
• HCM dimension conditions assigned to the sketch are taken over as parametric dimensions.
• If a preview of the revolved solid is displayed, it is only updated, in the case of changes to the values in the input fields, if you confirm the value input by pressing ENTER.
• If the sketch already exists, you can also use the Revolved part from sketch function in the context menu of the sketch to create the revolved part. Please note the following: If the sketch belongs to an assembly, the resulting revolved part will also be assigned to this assembly.

Dialogue Window for Revolved Solids • New Sketch • Part Creation Functions (3-D)