04. Constructing Base Features.pptx

SHEET METAL Constructing base features

Content :

SHEET METAL WORKFLOW ESTABLISH BASIC PARTCHARACTERISTICS DEFINE THE BASIC SHAPE OF THE PART CONSTRUCTING BASE FEATURES SHEET METAL CORNERS SHEET METAL CUTOUTS SHEET METAL DEFORM FEATURES FLAT SOLID AND FLAT PATTERN ADVANCED SHEET METAL COMMANDS ANALYZE FORMABILITY – ONE STEP AEROSPACE SHEET METAL WORKING WITH NON-SHEETMETAL DATA

CONSTRUCTING BASE FEATURES Purpose

Objectives

• This lesson introduces you to the following:

• Upon completion of this lesson, you will be able to:

• Sheet metal base features like tabs, contour flanges, lofted flanges, hem flanges, and jogs. • You will also learn how to create a sheet metal part from a solid model. • Bending and unbending in Sheet Metal. • Editing basic flanges.

• Identify key geometric elements necessary to create sheet metal base features like tab, contour flange, lofted flange, hem flange, jog, and so on. • Recognize the benefits of different types of base features. • Identify the key options in the Tab, Contour Flange, Lofted Flange, Hem Flange, Jog, Sheet Metal from Solid dialog boxes. • Create and edit sheet metal base features.

Tab • Use this command to construct a base Tab feature or to add material to existing faces of a sheet metal part. The following image shows the key components needed to create a base Tab feature. • A planar sketch or section string used for the profile. • A system-generated vector to determine material thickness and direction • Secondary Tabs display one vector to indicate the side of the profile where material will be added.

Tips for creating tabs • The base Tab feature must be a closed profile. • You can use an open profile for a secondary Tab. Any open profile must intersect the base feature at some point.

• It is recommended that you create section curves or sketch curves to include all required radii for your part. • Section curves can be either associative or non-associative to existing geometry.

• You can use the Add Existing Curves sketch option to create your profile, but you cannot create these curves using the Associative curve option.

Tab dialog box Type • Base Creates a base planar feature. • Secondary Creates a planar feature attached to another sheet metal feature.

Tab dialog box • Section

Sketch Section Lets you sketch a new profile from within the feature.

Curve Lets you select an existing sketch from which to create the profile. Thickness (Only available when Base is selected.) Specifies the thickness of the Tab feature. Secondary Tab features use the same thickness as the base feature.

Reverse Reverses the side of the profile on which the Direction Tab is created. Above the profile is the default.

Tab dialog box • Section

Sketch Section Lets you sketch a new profile from within the feature. Curve Lets you select an existing sketch from which to create the profile.

Thickness (Only available when Base is selected.) Specifies the thickness of the Tab feature. Secondary Tab features use the same thickness as the base feature. Reverse Reverses the side of the profile on which the Direction Tab is created. Above the profile is the default.

The following images show the components of two different construction options for secondary Tab features.

• A single profile sketch curve was used to add material to the corner.

•

An open sketch profile was used to extend the original base Tab feature.

Flange • Use the Flange command to add a flat flange at an angle to a planar face and add a bend between the two. • A flange consists of a bend region and a web. • = Bend region • = Web This command lets you:

• Construct simple bent or flanged areas and create an extension of the base feature to which the flange is attached. • Create complex flanges. To create these, you must edit the default flange profile sketch that is used to define the shape of the web portion of the flange.

Flange • Create sheet metal parts with internal flanges.

• Create flanges on bend regions.

• Create a flange on the edge of a deformed face formed by a Dimple feature. The edge of the deformed face must be linear, and the deformed face must be parallel to the original planar face on which the Dimple feature was created.

Flange dialog box

Editing Flange features •

Tips for redefining a Flange profile:

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In the Sketch Task Environment, use the Show/Remove Constraints option to remove any interfering inferred constraints that were created.

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Use the sketch trim commands whenever possible when editing the original sketch curves. This will help you maintain design intent by allowing you to keep the original curves and their relationships intact.

Contour Flange • Use the Contour Flange command to construct a flange by extruding a sketch along a vector, or add material by sweeping a sketch along an edge or chain of edges.

• You can: • Use the Contour Flange as the base feature of a new Sheet Metal part, or add the feature to existing Sheet Metal features. • Construct one or more bends at any angle. • Create a cylindrical contour Flange. This flange can be used to construct features that are wrapped around a cylinder, like parts made by rolling perforated material. • Use the Chain option to chain the Contour Flange around multiple selected edges. • Miter and close corners between the different Contour Flange sections.

Contour Flange • The following example shows a base Contour Flange feature. The bends are added automatically using the default bend radius value. You do not have to draw the arcs at each bend location. If you want to use a different bend radius value, you need to draw arcs in the section, or change the default bend radius value.

Contour Flange dialog box Type • Base Creates the Contour Flange feature as the base feature of a new Sheet Metal part.

• Secondary Adds a Contour Flange feature to existing Sheet Metal features.

Contour Flange dialog box • If there are no Sheet Metal features in the part, the command creates a base Contour Flange; otherwise, a secondary Contour Flange is created. • If the section for a secondary Contour Flange starts with an arc, it must be tangent to the face. • Section

Sketch Section Lets you sketch a new profile from within the feature.

Curve Lets you select an existing sketch from which to create the profile. • When you create a sketch on a path to define the section geometry, the location of the sketch defines the start location of the Contour Flange. Be sure to locate the sketch correctly along the path so that the Contour Flange is created in the correct location.

Contour Flange dialog box • Create a base contour flange 1. Choose Home tab→Bend group→Contour Flange. 2. In the Section group, click Sketch Section, and specify the plane on which you want to sketch the section geometry. 3. Sketch the open section. 4. In the Width group, from the Width Option list, select Symmetric.

Contour Flange dialog box 5. In the Thickness group, specify the thickness value. For this example, the default thickness of 3 is used.

You can modify the options available in the Bend Parameters, Relief, Miter, and Corner groups. For this example, the default values are used.

6. Click OK.

Lofted Flange Use this command to create a base or secondary feature between two sections, where the lofted shape is a linear transition between the sections. The two sections must be open and on parallel reference planes. You can:

• Create conical bend regions. • Add bends at each bend location using the Bend Radius option. •

You do not need to draw an arc at each bend location. Create transition regions between two different sections.

The following example shows the type of round-to-square transition that is used in HVAC technology.

Tips for creating Lofted Flange features • Section strings must be on parallel planes and must be open profiles.

• Only lofted flanges that consist of planes, partial cylinders, and partial cones can be flattened. • Any lofted flange that contains a ruled B-surface cannot be flattened. A B-surface face is constructed when: • The start and end section lines have a different relative angle. • Two section arcs have different start angles, end angles, or total angles. • An arc is mapped to a line.

Tips for creating Lofted Flange features • It is recommended that you create any fillet curve geometry needed. The inside bend radii must be greater than the material thickness for the Lofted Flange to be created. • Once you create an internal sketch for a Lofted Flange feature, you cannot reverse the creation method and make the sketch external to the feature. • At this time, it is not recommended that you use the Secondary Lofted Flange.

Jog • Use the Jog command to create an offset or a step in a tab. You can use small jogs to provide clearance or rigidity to a part. The section for the jog must consist of a single line across a planar face. • NX creates the jog by lifting material on one side of a sketch line and adding a flange between the two sides.

Jog dialog box

Jog Line

Select Curve lets you sketch a new profile from within the feature or select an existing sketch from which to create the jog line.

Jog Properties • Height Specifies the extent of the jog. • Reverse Changes the direction of the jog from up to down Direction and vice versa. • Reverse Changes the side of the part that moves to create Side the jog. • Height Reference Inside applies the dimension from the selected face to the near side of the feature. Outside applies the dimension from the selected face to the far side of the feature.

Jog Properties • Inset

Material Inside positions the portion of the feature that is perpendicular to the profile plane inside of the profile plane. Material Outside positions the portion of the feature that's perpendicular to the profile plane outside of the profile plane. Bend Outside positions both the portion of the feature that's perpendicular to the profile plane and the bend outside of the profile plane.

• Extend Section

Extends the linear profile you draw to the edges of the part.

Create a Jog To create a Jog feature on a tab, or a planar region of a contour flange or lofted flange: 1. Choose Home tab → Bend group → Jog .

2. Draw a profile or pick an existing sketch to serve as the Jog Line. The profile must be a single linear element.

Create a Jog 3. (Optional) Click on the drag handle to define the direction in which you want to create the jog feature. The drag handle should point toward the portion of the part you want to move. (The following figures illustrate the results produced by selecting different jog directions.) 4. Specify the height of the jog. 5. Click OK to finish the feature.

Bend • Modifies the model by bending material on one side of a sketch line, adding a bend between the two sides. • Bend dialog box

Bend • Bend Line

Select Curve lets you create the profile for the bend line. Sketch Section Lets you sketch a profile from within the feature. Curve Lets you select an existing sketch from which to create the profile.

• Bend Properties

Lets you define the shape of the Bend feature.

Angle Lets you specify the angle of the bend. This value must be greater than zero and less than 360 degrees. Reverse Direction

Changes the direction of the bend from up to down and vice versa. Reverse Side Switches the side of the part that moves to create the bend.

Inset Outer Mold Line Profile Specifies that the profile represents the line created by the junction between the planar stationary region and the cylindrical bend region in the flattened state.

Bend Center Line Profile Specifies that the profile line represents the center line of the bend, and that the bend region will be distributed evenly on either side of the profile in the flattened state. Inner Mold Line Profile Specifies that the profile represents the line created by the junction of the planar web region and the cylindrical bend region in the flattened state.

Inset Inner Mold Line Profile Specifies that the profile represents the line created by the junction of the planar web region and the cylindrical bend region in the flattened state. The image below shows the formation for the first three Inset options. The colored line at the bottom of the image indicates the plane of the sketch curve. 1: Outer Mold Line Profile

2: Bend Center Line Profile 3: Inner Mold Line Profile

Inset •

Material Inside Positions the portion of the feature that is perpendicular to the profile plane inside the profile plane.

•

Material Outside Positions the portion of the feature that's perpendicular to the profile plane outside of the profile plane. • Extend Section Extends the linear profile you draw to the edges of the part.

Create a bend on a tab 1. Choose Home tab → Bend group → Bend

.

2. Click Sketch Section to specify the plane on which you want to sketch the section geometry. For this example, the planar face of the Tab feature is selected. 3. Create the sketch to define the bend center line.

Create a bend on a tab 4. Click Finish Sketch to exit the Sketch task environment. 5. In the Bend Properties group: a. Angle = 60 b. Click Reverse Direction to reverse the bend direction.

c. Click Reverse Side to change the side of the part to move. The direction arrow points towards the portion that will move.

Create a bend on a tab 6.

Click OK to create the bend.

Unbend • Use this command to unbend a portion of the part to construct a cutout or a hole across the bend. You can then apply a rebend on top of the unbend feature to represent the true formed state of the model.

Unbend • Unbend non-uniform thickness bends that are created when you apply blends or chamfers, or create counter bored holes, countersunk holes, or tapered holes in the bend region. After the unbend operation, NX retains the features that you apply or create in the bend region. • The example shows a part modeled in the Sheet Metal application using features such as Extrude, Revolve, Draft, and Edge Blend in the bend region. These features are retained when you unbend the Sheet Metal part.

• Unbend non-uniform thickness bends that are created across conical bends.

Rebend Use the Rebend command to reverse an unbend operation so that the feature that was unbent returns to its previous bent state. Any features added after the unbend operation are properly repositioned during the rebend operation. You can: • Specify a face or an edge that remains stationary during the rebend operation, to control the positioning of the resultant body. • Rebend non-uniform thickness bends that are created when you apply blends or chamfers, or create counter bored holes, countersunk holes, or tapered holes in the bend region.

Rebend • The Rebend command lets you rebend individual bend regions that have previously been modified with the Unbend command. • Original sheet metal part • Part flattened using the Unbend operation • Normal Cutout feature added to the sheet metal part • After the Rebend operation, the Normal Cutout feature is also repositioned

Summary: Constructing base features • In this lesson you: • Learned about key geometric elements necessary to create sheet metal base features like tabs, contour flanges, lofted flanges, hem flanges, jogs, and so on.

• Identified the benefits of different types of base features. • Identified the key options in the Tab, Contour Flange, Lofted Flange, Hem Flange, Jog, Sheet Metal from Solid dialog boxes.

• Created and edit sheet metal base features.