Operations with the assembly

Let us insert a standard Angle from the Content Center. From a drop-down menu choose Place and next Place from Content Center or by clicking the right mouse button and choosing the same item.

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You see the window, where you can choose standard components. The left part of the window contains a tree structure, which contains all components, grouped into folders.

Click on the Structural shapes and choose Angles.

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You can see the angles for all set libraries. If we only need the GOST angles, we should apply filter and check the corresponding item: GOST.

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Select the angle GOST 8509-93. The resulting table contains all typical sizes of angles. We select angle 4 with leg thickness equal to 5. Enter the bar length 500.

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Press OK and save it as a new part.

Next insert it into our assembly.

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Using combining constraint, merge the angle with our Rack part.


Next select another option Flush and combine front faces of the angle and the Rack. Apply the constraints.

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In the context menu of the cube Set current vies as Front.

There are several operation to edit an assembly.

You can edit constraints applied earlier.

Let us edit an offset value for the Rib. To do this press on the plus sign in browser area and select the needed constraint. After selecting a constraint, you see that surfaces that were used to create it, are highlighted.

In the bottom of the browser area, you can see the offset value. In our case, it is equal to 246.

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Change this value to 10. We’ve inserted this Rib in our assembly, but we need to insert three such ribs.

We can separately insert each of them and specify the offset constraint, or we can make a pattern. On the Component panel, select Pattern. To choose a component we should specify a rib. On the Rectangle tab, we can select one from two pattern selection directions: columns or rows. We will need only one of them. Press on the column direction and specify the line for the pattern direction. We can select a line on any part.

After specifying a line, press on number of elements 3 and specify distance equal to 237.

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Now in browser area you see the icon of a pattern. You can edit it anytime you want.

In your assembly, you can also have construction geometry: planes, axis, and points. Let us create work plane on the back plane of our Angle.

Specify the back plane of the Angle, rib of the Angle and plane rotation angle equal to 0.

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Change the name of the plane to Wall.

You can make holes not only in separate parts, but also in an assembly. And they will not be displayed in the part file.

Let us create four holes in our rack. Go to the 3D model tab and press Create hole. Leave Linear placement. Select the top face of the rack to create holes in and specify the distance to the ribs. Bottom: 20 mm, left: 50 mm. Termination is Through all, diameter is 15 mm.

Press Apply and close.

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Now let us create a pattern of holes. Select Rectangle pattern, the element is our hole. Specify Direction 1, this is a linear rib. Change the direction. The number of elements: 2, the distance is 400. Specify the Direction 2: cross cut rib. The number of elements is 2, the distance is 100. Press OK.

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Now we have the pattern of holes.

Open the part Rack. Click on it with right mouse button and press Open.

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We see that created holes are visible only in the assembly.

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Let us make grooves in the angle. To do this we just extrude one groove and make a pattern.

Select Start 2D Sketch and select planes to create our sketch: back side of the angle.

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When creating a sketch of the assembly, it does not have any projected lines of the selected part. Press Project Geometry and select the necessary ribs.

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Using the Line function draw our groove. We draw a horizontal line, than the cursor to the end of the line, until you see the gray dot, click left mouse button and draw an arc, next draw one more line and one more arc.

Specify the sizes of our groove. The radius is 7 millimeters, distance between central points of the arcs is 16 millimeters. Distance from the bottom of the angle to its center is 20 millimeters, and from the side of the angle to its center is 14 millimeters.

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Apply sketch. Select the operation Extrude. Select the groove and specify the distance To. Select the back side of the angle and press OK.

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In the browser area all procedures with the assembly are displayed separately from the parts, in the beginning of the list.

Rename Extrusion 1 to Groove. If needed, double click to edit an operation or a sketch.

Press on Rectangular pattern. Select the element Groove, specify the direction of the pattern and input distance 228 millimeters, number of elements is 3. Press OK.

Now we have a pattern consisting of three grooves.

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It is important not to misunderstand the pattern of elements on the tab 3D Model, which deals with a pattern of elements, and not to confuse it with the pattern of components, which is responsible for the creation of the pattern of parts and components.

Open the part Angle. You can see that grooves did not appear on the part and are visible only in the assembly.

On the Manage tab, you can view the specification of the current assembly. It contains the name and the amount of all inserted parts, along with the length of inserted standard profiles.

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You can add various data to the table through the Customization option. Add the mass property.

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Save the assembly, close it and its parts.

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