Creating Tooth of Hacksaw Blade-Autodesk Inventor 2013 (with caption and audio narration)
Serial No. 193 Creating Tooth of Hacksaw Blade-Autodesk Inventor 2013 (with caption and audio narration) In this exercise we have used two 3D features → Extrude (Cut operation) and Rectangular Pattern. Here a pre constructed part ‘Blade’ is taken from the model ‘Hacksaw’. Click the following link to get the model file: – http://bit.ly/2ooUYmN Transcription of Video Open the Blade (.ipt) file. A pre constructed Blade part file is visible in isometric view. Select blue face of the Blade. When the mini-toolbar appears, click the third button on the right, labeled with the tooltip Create Sketch. Now we are in the sketch environment. Take the project of the model by using Project Cut Edges tool. Select all the sketches in the design window and convert them into construction geometry. Create tooth profile with the help of line tool. Now the sketch is complete. Finish the 2D sketch. Select any line of the enclosed profile, the mini-toolbar appears in the graphics window. Click the Create Extrude icon. It will automatically select the tooth profile. Extrude dialog box is visible in the design window. In the Extents field, select ‘All’ option from the drop down list. It will automatically select the ‘Cut’ operation. Click OK to create the feature. Click the ‘Rectangular Pattern’ icon on the Pattern panel of 3D Model tab. Rectangular Pattern dialogue box is visible in the graphics window. Features button is active by default. Select Extrusion3 from the browser bar. Right click in the graphics window and choose Continue. Select horizontal edge of the blade parallel to X Axis to define the direction of pattern. Choose the Flip button to reverse the direction. Set the column count to 192. Set the column spacing to 0.0625 inch. Now the preview of pattern is visible. Click OK to execute the Rectangular Pattern Feature. Right click the Rectangular Pattern2 in the browser bar, and then select Show Dimensions.
Application of ‘Text’ tool and ‘Emboss’ tool-Autodesk Inventor 2013 (with caption and audio narration)
Serial No. 192 Application of ‘Text’ tool and ‘Emboss’ tool-Autodesk Inventor 2013 (with caption and audio narration) In this exercise a pre constructed part file ‘Anvil’ is used. Click the following link to get the model file: – http://bit.ly/2nJyMTG Transcription of Video Open the Anvil (.ipt) file. At present a pre constructed part file of ‘Anvil’ is visible in the isometric view. Create a new sketch on the blue face of the Anvil with the help of ‘Create 2D Sketch’ tool. Take the project of the model by using ‘Project Cut Edges’ tool. Select the projected model edges in the design window and convert them into construction geometry. Start the ‘Text’ tool from the Draw panel of the Sketch tab. In the graphics window, click to place the insertion point for the text box and drag to define the area of the text box. Format Text dialogue box is visible in the graphics window. In the ‘Format Text’ dialogue box, enter the text ANVIL in the specified area. Select text and choose Center Justification and Middle Justification in the ‘Style’ option. Enter the value 0.8 in the ‘Size’ field. Change the text colour to Red. In the ‘Font’ field, select ‘Calibri’ font from the drop down list. Click OK to place the Text. Right click in the graphics window and click OK to finish the command. Apply Vertical constraint and Coincident constraint on the text to position it properly. Finish the 2D sketch. Activate the ‘Emboss’ tool from the Create panel of the 3D Model tab. Emboss dialogue box is visible in the design window. The profile selection is activated by default. Select text as profile. In the ‘Depth’ field enter the value 0.25 inch. Change the direction of the feature by clicking the flip direction button. Click OK to execute the Emboss feature. Select the Emboss feature in the browser bar and activate the ‘Adjust’ tool from the ‘Quick Access Tool Bar’. Adjust the appearance tinting of the feature and click OK to apply.
