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Sunday, November 16, 2008

Bolt & Nut - Threading

Mechanical Design > Part Design

In this tutorial I'm going to show how to make bolt and nut that will involve threading.

Open the Assembly Design Workbench because we are going to create both bolt and nut and will assemble them together.

In the Workbench, right-click on the Product1 tree and select properties. When the Properties box appeared, rename the Part Number to Bolt&Nut and click OK. You'll see the Product1 name had been changed to Bolt&Nut.



Then right-click on the Bolt&Nut tree and select Components > New Part. As the new part has existed, expand the tree and select the properties of the new part. Rename both the Instance Name and Part Number to Bolt as shown in the figure.





Now double-click on the xy-plane and we'll be automatically switched to the Part Design Workbench. Then select the Sketcher tool to make the first drawing. In the Sketcher Workbench, select the Hexagon tool. (click the arrow below the Rectagle tool to view the Hexagon tool) or select Insert > Profile > Predefined Profile > Hexagon. Then resize the hexagon using the Constraint tool at the circle surrounding the hexagon. Adjust the diameter value int the Constraint Definition box to 30mm.



After done with the hexagon, exit the Sketcher Workbench and make a pad from the Sketch.1 with pad length of 10mm. Make sure u select the Reverse Direction button as shown in the figure.



Done with the pad, select the lower surface of the part as shown in the figure and use the Sketcher tool again. Create a circle at the center of the hexagon with a diameter of 16mm. Then exit the Workbench and make another pad from the Sketch.2 with 50mm pad length.





Now we are going to insert some thread to the bolt. Click on the Thread/Tap tool or select Insert > Dress-up Features > Thread/Tap. A Thread/Tap Definition box will appear and enter values as shown in the figure below.



*Note. The thread will not be visible unless in the Drafting Workbench.

Now we are making the nut.

Right-click on the Bolt&Nut tree and insert New Part. Rename it to Nut.
Create a part with similar method as above except for the second sketch (Sketch.2) the diameter is 15mm and make a pocket instead of a pad. Values for threads are as same as above.



Double click on the Bolt&Nut tree to activate the Assembly Workbench. Use the Manipulation tool to move the nut and bolt together as shown in the figure.



With the Bolt&Nut still selected, select Start > Mechanical Design > Drafting. Just click OK when the New Drawing Creation box appear.



Click on the Front View tool or select Insert > Views > Projections > Front View. Then select the window toolbar and select the Bolt&Nut.CATproduct (switch to the Assembly Workbench view).
Then select a flat surface of the bolt to be the front surface for the drafting. Then rotate it to a suitable view.



Right-click on the properties of the Front View projection and check the Center line, Hidden Lines, Axis, and Thread.





*Note: Thread shown in this view is according to the Standard of CAD Drawings.




3 comments:

veva said...

Hello..
thanks for coment my blog "scorpio".
Take care

Anonymous said...

you rock bro!

Lawrin Francis said...

thnx it helped me a lot!

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Catia V5 Tutorial by Ridhuan Othman is licensed under a Creative Commons Attribution-Share Alike 2.5 Malaysia License