Sweep Part (3-D)

3-D Standard > New > C-edge sweep

You use this function to create a 3-D part by placing cross-sections on 3-D guidelines.

• The guideline can be a sketch, a 3-D sketch or a hyperedge. Curved guidelines are also allowed.
• The cross-sections must be sketches.

Proceed as follows:

1. Activate the function either via the Ribbon or via the context menu for parts. Please note that you can insert the part as main part or as sub-part.
2. Enter the Part name of the new sweep body.
3. Activate or deactivate the Reference and Feature and BOM-relevant checkboxes.
4. Under Type, choose whether you want a solid or hollow body to be created.
5. To create a solid body, you need to deactivate the Hollow checkbox.
6. To create a hollow body, activate the Hollow checkbox and enter the desired wall thickness. If you want the wall thickness to be marked off outwardly, also activate To outside.

5. Specify the type of cross-section you want to be placed:
6. Circular cross-section with a freely definable diameter
   Activate the Circular cross-section option and specify the diameter you want.
7. Arbitrary cross-section - based on a 3-D sketch
   Activate the Arbitrary cross-section option. If you want to define the direction for the placing, then also activate the With With direction specification option.

6. Identify the guidelines. To do this, click the Select guideline icon. All identified guidelines are entered in the list box of the dialogue window.

If you use two guidelines, you can select the following options from the Scaling list box in the Type area:

• Evenly
  Places the sketch between the two guidelines, scaling the cross-sections evenly in both directions.
• Retain height
  Places the sketch in such a way that the height of the cross-sections corresponds to the height of the original sketch.
  
• Retain cross-section
  Places the sketch in its original size, i.e. the cross-sections placed on the guideline have exactly the form and size of the identified sketch. The cross-sections will be attached to the points of the first guideline and placed in the direction of the second guideline.

Scaling options, 2 guidelines: (1) Evenly, (2) Retain height, (3) Retain cross-section

7. If the With direction specification option is active, then specify the direction after identifying the guidelines. To do this, click the Specify direction vector icon and the define the vector by specifying two points or by identifying an edge.
8. For arbitrary cross-sections, now specify the relevant 3-D sketch.
   If you want to create a new sketch, then click the New sketch icon. Next, use the sketch functions to construct the desired cross-section.
   If you want to use an existing cross-section, click the Select sketch icon and identify the sketch you want.

If the Position sketch automatically option is active, the cross-section is placed in the plane vertical to the first identified guideline edge so that the fitting point of the cross-section lies in the start point of this edge.

If you want to position the sketch differently, click the Move sketch icon after creating/selecting the sketch. You can then still rotate, move or mirror the cross-section before placing it.

9. If you want to check initially what the created part looks like, click the Preview button and then Apply if you want the part to be created as displayed. If you want the part to be created directly – without preview –, click the Create button.

If you want the sweep part to be inserted as sub-part to the active part, click and select Create new c-edge sweep as sub-part .

 Related Topics

Place Circular Cross-Sections (3-D) • Place Arbitrary Cross-Sections (3-D) • Sketch Functions (3-D)