Task with parts

There is a range of tasks in order to edit parts. Let us review some of them.

First, let us open Part 2 we’ve created earlier.

The software allows us to assign parts of the properties of various materials. Right click on the part name (in the browser area) and select Inventor Properties. On the tab Physical you can see the current materials: volume, density, and mass.

You can choose from any available materials. We select Steel, Carbon.

You see that the density and mass of the part have changed.

If needed, you can specify any texture of the material. In the dropdown menu, while selecting color, choose SteelCast.

 

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The texture of the part has changed.

Now let us review options for specifying holes. Choose the Hole function.

Leave linear placement. Specify the starting face of the hole and choose edges to link the position of the hole:

 

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Enter 15 from the first edge, and 10 from the second.

We can specify various configurations of the hole: either simple hole, or screw hole.

As a limit, we can choose either Distance or Trough all.

We choose simple hole with a diameter of 6 mm Through all. We got the hole to correspond to the specified parameters.

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The second way to get a hole in a part is via a pre-drawn sketch.

Let us start a sketch on the face-side of the part. Place three points, and specify Vertical constrain between them. Specify the distance between the points, and the distance from the bottom point to the edges. Finish Sketch.

Select the Hole task and the holes are immediately placed where the points are.  The placement is specified as From Sketch.

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By clicking the dot in the center while holding the Shift key, you can cancel the selected points.

Select the screw hole with chamfer.

Type of screw – ISO metric. It corresponds to the size of the screw according to the National State Standard. The size of the hole is М6. Select the Distance termination and specify the chamfer diameter as 8 mm.

Set the depth of the hole as 25 mm, the depth of the thread is 20 mm, and press OK. Now we have the holes, placed by the created sketch with the specified parameters.

 

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Save the part.

You can create chamfers and fillets on the part itself.

Let us create a chamfer for the first hole. Specify the distance equal to 1 mm, choose the edge. Apply.

 

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Now choose the Thread operations and specify the thread for the first hole.

Select the edge.

 

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On the Specification tab choose ISO metric profile, size is M6. We can choose the direction: either right hand, or left hand. Apply.

Select the Fillet task.

As working edges, we choose the top edges of the part.

 

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On the Constant tab, you can specify the radius of the fillet. Set it to 4 mm, press OK.

Direct Edit operation is used to change the geometry of the part.

Let us move the top face by 10 mm. Choose the Direct Edit, select the top face. You can regulate that movement. We input the exact value: X=0, Y=0, Z=10.

 

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You can check the size of the part on the tab Inspect, then Distance feature. You can select the distance between faces or edges. Moreover, you can inspect the distance to the holes.

 

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Using the Pattern task, you can create a rectangular or circular pattern of elements. For example, let us select the rectangular pattern and choose the following elements: first hole, chamfer, and thread.

 

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As a direction, you may choose any face, but it is better to choose a plane of the part. As a direction, we choose the XY plane. Here the number of elements is two; the distance is 15 mm.

We got the two holes with distance 15 mm between each other.

 

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Save the part.

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