Catia v5 Tutorial: Shaft and Hole

It has been quite a long time since my last post. In fact, it has been two years. Anyway, I am back and I hope to pick up from where I left off from the last post.

Instead of making a continuation of the last project, I have decided to start anew. Therefore, this post will be on getting familiar with the Shaft and the Hole  tool.

In this Catia project, we will be aiming to create something similar to this part:

Open up Part Design and let's name this part as Bearing Socket.

First of all, we will create a sphere with a diameter of 4-inch. In order to do that, click the Sketch tool and select the yz plane. In the workbench, select the Arc  tool which is located in the extension under the Circle tool.

 

Now draw half a circle and close the arc with a straight line like so:

Exit the workbench and select the drawing that you have just done. Select the Shaft tool and a Shaft Definition window will pop-up. Under axis selection, select the vertical straight line of the half-circle and then click "OK". A sphere should have been created.

Next, click the Sketch tool and select the xy plane. Draw a circle with a 2-inch diameter right next to the sphere that you had previously created. This circle can be drawn anywhere on the screen but preferably somewhere nearby the sphere. Now click the dot at the center of the circle and while holding on to the "Ctrl" button on your keyboard, select any surface of the sphere. Holding down the "Ctrl" button allows you to select multiple elements.

Select the Constraints Defined in Dialog Box tool   and select Coincidence. This will automatically align the center of the circle to be coincident with the center of the sphere.

Exit the workbench and click the Pad function. Select the circle and in the Pad Definition window, change the Type to Up to Next and hit OK.

Create a 4-inch Edge Fillet at the edge at the joint connecting the cylinder and the sphere.

Enter sketcher mode on the xy plane again. Create a 5-inch by 2.2-inch rectangle. Use the Contraint   tool to align the rectangle as shown in this picture:

Exit the sketcher mode and select the Pocket tool. Under the Type in the Pocket Definition window, select Up to Last, click the Reverse Side button and click OK. You will end up with a part which looks like this:

Click the Hole tool and select the edge highlighted in red, followed by the surface which is labeled as "A".

A Hole Definition window will appear. Under the Extension tab, select Up to Last and set the diameter to 2-inch. This is what your part should look like:

Get into Sketch in the xy plane and draw a hexagon with a diameter of 3-inch.

Select the dotted circle around the hexagon and the circle of the cylinder at the same time. Select the Constraints Defined in Dialog Box tool and select Concentricity.

Exit the workbench and select the Pad tool. In the Pad Definition window, set the Length to 1-inch.

Select the Hole tool and select the bottom surface of the hexagon. In the Hole Definition window, select Blind and set the Diameter to 1.5-inch while the Depth to 3-inch. Next, under the Type tab, select the Counterbore option. Set the Diameter to 1.7-inch and Depth to 0.3-inch.

This is how the inside should look like:

And our simple bearing socket it finally done. This picture will show the 3-view picture of the bearing socket that we have just created.

I hope that you found something useful in this tutorial. Make sure to check back for future updates in Catia v5 Tutorial for Beginners.