A concept of the project, parametric part

Inventor contains project files. Any project determines the position of all files, related to this particular project. In other words, project file defines all files, which are included in a particular product and excludes loss of connections between parts, assemblies, and sketches.

Let us create a new project. Press Projects and you will see the list of available projects.

 

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Press New. If you are using vault to store all your data, you can choose New Vault Project. If you are working on a separate computer, please choose New Single User Project. Press Next.

Specify the name of the project file Inventor tutorials and specify the path to the project files folder.

Libraries should be left without any changes.

Press Finish and a new project is created for you.

Let us create a new part. When you create a part, it is created in the current project in the specified folder.

We will make this part parametric, which means that management of the part sizes will be carried by parameters.

On the Manage tab choose Parameters.

 

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Here you see all the parameters of the model along with user-specified parameters.

Let us add user numeric parameters.

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Name our first parameter L1. In the Equation column enter 200, and in Comment field write line 1.

Create one more parameter L2, Equation is 300, comment is Line 2.

Third parameter should have a name H1, Equation is 10, in comment write Height.

Next create a parameter D1, Equation is 8, Comment is Diameter.

One more parameter LD1, Equation 15, Comment is To hole 1.

And the last parameter is LD2, Equation is 20, Comment is To hole 2.

Close the parameters window.

Let’s draw a rectangle in our sketch. With the help of Horizontal and Vertical constraints align it to the origin.

As distance of horizontal line input L1.

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As distance of the vertical line input L2.

Now the sides correspond to the entered parameters L1 and L2. Finish sketch.

Change the name of the part to Parametric and save it.

Choose the Extrude tool. As a distance enter H1.

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Press OK. The sketch is now extruded for the distance equal to H1, specified in the parameters.

On the front side of the part, we create a sketch. Place 4 dots, which will define the centers of the holes. Mutually align all the holes with the help of horizontal and vertical constraints. Define the dimension from the point to the rib equal to LD1. The second dimension is the same as the first one.

Dimension from the side rib is LD2. The last size is the same. Finish sketch.

 

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Next, select the Hole operation. The holes are located on the points of the sketch. Select the termination Through All. As a diameter, specify the D1 parameter.

 

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Press OK and you see the created hole with the diameter equal to 8 millimeters.

With the help of distance measurement, you can ensure that the sizes of the parts are equal to the entered parameters.

If you go the Manage Parameters you can see that besides User Parameters, there are also Model Parameters, which are assigned separate user-defined parameters.

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Let’s make the part parametric, i.e. specify different sizes for different versions of the same part.

On the tab Manage find Author and choose an item Create iPart.

In the resulting window, you can see the row for the first version, which already contains User Parameters.

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Here you can add other parameters or delete an unnecessary ones.

Let us create one more version of this part. To do this, right click on the row number and choose Insert row.

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Now we have the second row with the same parameters, but now they can be edited.

Input: L1 = 250, L2 = 250, H1 = 15, D1 = 12, LD1 = 25, LD2 = 25

Insert one more row for the third version.

This time input: L1 = 300, L2 = 450, H1 = 20, D1 = 15, LD1 = 40, LD2 = 30

 

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Press OK.

Now you see that in browser area, the icon for this part changed to the icon for parametric parts, and now it has the table of versions.

Open Inventor properties and on the tab Physical specify the material Steel Carbon. Now we can find out the mass of the part.

Double click to choose the second version.

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If you open the iProperties, you can see the results for mass calculation.

Select the third version to ensure that mass for this part has also changed.

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Save the part.

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