Project: HiCAD 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.
Proceed as follows:
Activate the function either via the Ribbon or via the context menu for parts. The New c-edge sweep dialogue window will be displayed.
Step 1: Specify type
To create a hollow body, activate the Hollow checkbox and enter the desired wall thickness. If you want the wall thickness to be applied to the outside, also activate the To outside checkbox.
To create a solid body, you need to deactivate the Hollow checkbox.
Activate this option if you want to create a circular cross-section. Enter the desired diameter.
Activate this option if you want to create an arbitrary cross-section based on a sketch. Depending on the number of selected guidelines, further options will be available in the listbox.
Step 2: Specify guidelines
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Select guidelines To specify the guidelines, click on the Select guidelines symbol and identify the desired guidelines in your drawing. All identified guidelines will be entered into the listbox in the dialogue window:
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Remove guideline from lists If you want to remove any guidelines from the list, click on the Remove guideline from list symbol and identify the corresponding guidelines in your drawing. |
Step 3: Select guideline-dependent options
Depending on the number of selected guidelines, further routing options will be available in the listbox below Type:
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1 guideline |
For 1 guideline, the following options are available: Minimum rotation This is the default setting. The sketch will be routed as evenly as possible and with minimum rotation along the guideline. Please note that the available degrees of freedom are limited here. If the guideline is not located in one plane, this may lead to unwanted contortions (genuine 3-D). Direction specification This option enables you to determine the direction of the routing by specifying a direction vector. The cross-sections will then be aligned in the direction of the vector. You can either specify the vector by selecting 2 points, or select the edge direction. The tangent of the guideline must nowhere run parallel to the direction specification. If, for instance, the guideline is a spiral, and the spiral axis is the direction, sections through the sweep part with a cut plane containing the spiral axis would result in constant cross-sections (Examples:spiral ascending parking garage drive, screw thread). Constant angle with direction Here, too, routing takes place by specification of a direction vector. You can either specify the vector by selecting 2 points, or select the edge direction. In contrast to the Direction specification option, the routing will take place with a constant angle. If, for instance, the guideline is a spiral, and the spiral axis is the direction, sections through the sweep part and perpendicular to the guideline would result in constant cross-sections which are not twisted laterally around the guideline (Examples: Routed profiles, staircase handrails). The tangent of the guideline must nowhere run parallel to the direction specification.
Click here to see further examples. |
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2 guidelines |
For 2 guidelines the following options are available in the Scaling listbox: Evenly
Places the sketch evenly between the two guidelines. The placed cross-sections will be scaled evenly in both directions relative to the original sketch. Retain height
Places the sketch between the two guidelines 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 original size, i.e. the size and form of the cross-sections placed along the guideline correspond exactly to those of the identified sketch. The cross-sections will be attached to the points on the first guideline and placed in the direction of of the second guideline. |
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3 guidelines |
For 3 guidelines, the routing takes place evenly between the guidelines. The placed cross-sections will be scaled evenly in all directions relative to the original sketch. |
Step 4: Select / draw sketch
If you have selected the Arbitrary cross-section in the Type area, you now need to identify an existing sketch, or draw a new one.
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Create new sketch If you want to create a new sketch for the cross-section, click on this symbol. Then, draw the desired cross-section using the Sketch functions. |
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Select sketch If you want to use an already existing sketch for the routing, click on this symbol and identify the desired sketch. If the |
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Position sketch If you want to position the sketch in a different way, click this symbol after creating/selecting the sketch. You can move, rotate or mirror the cross-section before placing it. |
Step 5: Article number and further options
In the Article number input field, enter the name of the new sweep body.
Depending on your requirements, activate or deactivate the Reference, Feature and BOM-relevant checkboxes.
Step 6: Check / start routing
If you want to check what the part to be created will look like, click the Preview button. Click Apply if you want to generate the part as displayed in the preview. To start the actual generation of the part, click the Create button.
Please note:
and select Create new c-edge sweep as sub-part 
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Place Circular Cross-Sections (3-D) • Place Arbitrary Cross-Sections (3-D) • Sketch Functions (3-D)
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If the guideline is located in one plane and the surface normal is selected as direction, the options will produce identical results when the sweep body is created. 
